Six or so months ago there was a thread on this forum featuring a fellow who set up various lathe tools and drill chucks on a plate mounted in vises on his mill table. He put bar stock into the spindle and used the mill to perform limited lathe functions. I have not been successful finding it with the search function, does anyone remember it?

I haven't seen that thread, but I have done what you describe on several occasions, and Have an old video around somewhere of one of my setups.

Here is a YouTube vid of that type of thing being done in a small Taig benchtop.
http://www.youtube.com/watch?v=wbfXXeiSHsw

I haven't seen that thread, but I have done what you describe on several occasions, and Have an old video around somewhere of one of my setups.

It is buried somewhere; I think I even posted to it but that would be buried about a year back or more. What was interesting was the person doing it was making bushings or spacers on a production basis very successfully.

That might have been me. :) Here's a video of mine running. http://s207.photobucket.com/albums/bb180/matt_rfr/?action=view&current=Latheonmill.flv

Very cool! The last thing I did like that was use a drill press as a lathe to turn a handful of bushings. I clamped a brazed carbide lathe bit in the vise and used the quill stop for length.

That was the last mickey-mouse setup I did before buying a real lathe and mill.

Hi Vern,
I remember the one. I'm still looking for it.
I knew hoss did one http://www.cnczone.com/forums/showthread.php?t=30385&page=8
I was thinking of having a block along the front of the table.
Say 3" or more high, cut slots in it to fit all your tooling in.
Then just move along to the next tool to use it.

Rod

Threading on a mill (video (http://www.centroidcnc.com/cncvideo/video_threadmill.html)).


.

I think the one I remember was Matt@RFR. Anyhow, this has been a great thread, lots of ideas for my set up. I need a bunch of simple aluminum flange bushings of various IDs, OD's, lengths, and shoulder widths. I think a set up like this will work fine without spending thirty grand on a CNC lathe. I have enough old lathe tooling and drill chucks laying around to make it. I doubt if I'll ever have enough turning work to justify a CNC lathe.

If I get it to work I guess I'll have to invest in a digital movie camera to post pictures of it in action. :)

If you go and look around the KBCtools website you should be able to find a very nice little three jaw chuck that is small enough to fit on a CAT40 toolholder; they come with a 5C shank but are bolted to a flange so it would be a simple matter to make an adapter. Cost is around $280.00 I think and includes two sets of jaws for ID and OD clamping. For doing semi-production work I think it would be feasible to have two chucks; one with a part in the machine being processed the other being reloaded.

And a thought cam to mind: How would you cut a thread using a mill as a lathe?

How does someone program something like this? This looks like an ideal solution to some of my needs, but i'm lost on how to accomplish it with the CAD/CAM software.

Can anyone who has done it give some tips on how to go about doing something like this???

Thanks,
Wade

That's a good idea. I was thinking about using collets and coming up with a way to loosen and tighten the collet nut without using spindle orient to hold it. I'm sure locking the spindle with spindle orient would not go over well with Haas.

Do you think the little chuck would be OK at 2000 RPM from a balance standpoint?

Vern

For programming my initial thoughts were using multiple work offsets ( G54, G55, G56 etc.) for each tool station. The offsets would then be moved between operations to determine the amount of material that would be removed in each vertical pass.

The vertical component could be handled with various drilling and boring functions I would think. I'm sure this would be a great place for Goef's G12 use if anyone can figure out how. :)

I hope some of you smart guys will find this interesting enough to comment on since I've never done it.

Vern

Just program X and Z almost the same as on a lathe. I find to get myself oriented I have to stand at the machine and put my head to one side. I think to get the sign on X correct; i.e. negative being toward the spindle centerline, the spindle has to rotate backwards. I have written MDI programs to machine clearance tapers and steps on the end of tool holders and seem to remember that something has to go backwards.

Regarding your offsets for each tool I think that would work fine, I only ever used one tool at a time. For the vertical offset I think this could probably be in the Z entry of the main offsets. It is an interesting exercise trying to visualize it without a machine around; I have the gut feeling that it should be possible to configure things so it was almost the same as a lathe program. Lathe tool numbers and offsets are substituted by work offsets.

Starting into CNC in February I have little experience and have used CAM software almost exclusively. My hand coding has been limited to editing posts on the machine. I've never programmed a lathe, CAM or hand, so I'll probably fall on my face a few times before I get this figured out. Just want to be sure I don't crash, probably use a wooden dowel in the spindle for a while. :D

For my chuck, I bought a Bison 3" (can't remember the cost) and it's good for 4,000 rpm. I bought a 1.5" endmill holder and made an adapter to bolt the chuck to. I don't like this setup only because it's so damn long @ 7" gauge length. But it does work. 3/4" and under raw material I would use several collet holders and run as many as I could as I was reloading outside the machine. One thing to consider though is it took me VERY little time to reload that chuck...I would rapid up maybe 8" in Z, then M19 Pxx.x so the chuck wrench would be where I wanted it. M30 cancels M19 but it stays put.

As far as programming is concerned, it's very basic. You can still use drill cycles like normal, you need to be in G18, G2's and G3's are backwards but I and K coordinates are in the standard direction. That's the worst part. Ofcourse this all depends on how you have your tooling oriented and which side of the tool you're on. I've got mine with the insert nose pointed to the right (X+) so to feed in to the part, it's an X- move. That ends up being just like a lathe in that X zero is the center of the part.

I started out hand programming this setup, but quickly found that without tool comp I couldn't quite wrap my head around how to alter the tool path to get the radii sized correctly. Mastercam handles that nicely with computer comp, but using CAM opens up other obstacles. The worst of which for me is having to divide each and every X number by two. This depends on your post processor and how you have your CAM software setup.

You will use one tool offset for length of the blank only. Everything else is handled by work offsets for each tool. The way I set mine is to probe everything in Z, then set X like you would in a lathe with no tool probe (skim OD, measure, offset by half OD). To set Y, I simply made facing passes and adjusted til there was no tit left. Not ideal, but I wasn't sure how else to do it. My setup has a bore in the top left of the big plate that I probe for G54, and all other offsets I enter by hand relative to that. I have everything written down, so the only offsets I ever need to change are the X for the parting tool and Z for drills and boring bars.

I'm attaching the program that was used to make the video I posted. It's been optimized (dropped like 20 seconds off the cycle time), so it's not exactly the same, but you'll get the idea.

Matt

Thanks for the millath information. :) I brought the subject of mounting a small lathe chuck onto a mill spindle up on another forum and Forrest Abby suggested using a CAT 40 shell mill arbor. I think this would get rid of some of the extra Z length you are dealing with.

Are you using lathe CAM software or mill? I've never programmed a lathe so I don't understand where G18 would get into the picture. From your video it looks like you have mounted your turning tools on the X minus (right side ) of the tool plate pointing toward the right side of the mill. If this is the case I would assume an X plus move would send the work into the tool which seems to be opposite what you are describing. Either I've miss read the video or my lack of G code knowledge for lathes is the problem.

I like the idea of working off the side of the tool plate because it keeps the tools more solidly mounted than putting them up on pedestals would. You also have access to the extra Z depth from the top of the tool plate to the top of the mill table.

I'll look over the program and maybe all of this will make more sense, thanks again.

Vern

G18 makes G02, G03 active in the X, Z plane.

For you holder you can get an ER32 from Iscar (I think that was the supplier, I will check) that is very short. I think you could make and adapter even shorter than would be possible with a shell mill holder. Here is a picture.

Vern, remember that you're moving the spindle, NOT the table, even though the table is the thing that moves. So X+ moves the table to the left. With that in mind, re-read that part of my post and I bet it makes more sense. :)

Geof, do you think an ER32 collet would be very rigid? That's the only reason I didn't go that direction originally, although with the gauge length I ended up with, I probably lost as much or more rigidity over a collet. I'm also liking the shell mill holder suggestion. In my video, I only had .75" or so clearance over the drill, and if I ever mistakenly put a tool change in the program (don't say it can't happen!), it would not be pretty.

I can see this is going to be a crash course in G code for me. I've always left the X, Y, +, and - stuff to the CAM software. :) Are all the turning tools mounted at zero rake allowing different inserts to handle rake angles and such?

Matt; I think a collet would be rigid enough; my reasoning is that you could snug the chuck up very close to the nose of the collet. The backplate only needs to be about 0.4 to mount the chuck and this can have a stem just over 3/4" to fit in the largest ER32 collet; you could even have a hole through it to do small, short bar work. The end of the chuck jaws would be no further from the nose of the collet than a standard 3/4" end mill and the cutting load being experienced is a minuscule fraction of what you would put on an end mill. One thing am sure of is you would have a much shorter mount using the holder I pictured compared with the shell mill holder.

Vern; Twist your point of view...pretend you are sitting on the spindle, well on the headstock I guess so you don't get dizzy :). Imagine the table coming up to you, not you going down to the table. So table upward, i.e. toward the chuck, is negative Z; if you have your tools positioned correctly tool movement toward the spindle centerline is negative X so it is the same as lathe programming.

The easiest way for me to not get confused is to picture moving the spindle in X and Y, not the table. It's exactly like a manual mill with a DRO if you have it set correctly.

Here's a picture of my toolholder. Hopefully it'll clear some things up some. And if it doesn't, yes, all the toolholders are set in the machine with zero rake, and the insert pocket and the inserts themselves take care of the rest of the geometry.

Geof, I never thought about endmills having a much greater load on the tool holder than a lathe tool would put on it, good point! Collet it is if I ever get around to it. If I end up using this more than a few times a year I definetely need to do something else with the chuck.

Can you set work offsets relative to G54 with a macro?

.....Can you set work offsets relative to G54 with a macro?

You probably can but you don't need it; use G52.

G52 gives you a local work zero with reference to the currently active work zero. Say you have G54 at -10.0 in X and -5.0 in Y and you give the command G52 X2.0 Y2.0 now your effective work offset is located at X+2.0 Y+2.0 relative to the G54 location and the command G00 X0.0 Y0.0 takes you there. In machine coordinates this is -8.0 in X and -3.0 in Y, you have displaced your main work offset over to here, temporarily. Whenever the machine calculates a coordinate position the values in the G52 register are added to the current work offset values.

For using the mill as a lathe I am not sure this is helpful but maybe it could be; you can also include Z in the G52 command so you could use G52 for both the location and length of all your tools, however you can do the same just using G54, 55, etc. And you can dynamically change the main work offsets in the program using G10 L2 G90 Pn Xx Yx Zz.

I was thinking about my statetement about lower cutting load and I am not entirely correct, you could be turning on a much larger diameter than 3/4", A 3.4" diameter part with a tool engagement depth, width and feed per rev, one tenth that of a 3/4" mill would give the same spindle load; the torque is the same. But it would not be giving the same bending load on the holder??? I think. However, I don't think this diameter of part is likely to be machined.

I've been looking over Matt's code and could only find G2 used in two places, line 44 and line 117. If I'm understanding G18 it put circular interpolation on the ZX axis, meaning that in helical milling the linear movement will be restricted to the Y axis rather then Z as normal. Matt used it both times on what he describes as "finish major OD" and "finish bore". I can't seem to envision what is happening here. I would think the effect of G18 on a millath would be the ability to cut a taper.

G03 on line 44, G02 on line 117.

Line 44 is going from a smaller diameter to a larger with a concave fillet; line 117 is going from a larger diameter to a smaller with a convex fillet. Both seem logical for lathe programming.

This circular interpolation is in the X Z plane so you need to use G18 on the mill to make the commands active in that plane. It is not equivalent to helical milling. Using the mill as a lathe you are not moving Y.

In helical milling the G02/03 is in the X Y plane and the Z motion is a separate linear motion that moves the Z distance during the time needed for the X Y circular interpolation.

Got ya, so it's radius-ed taper. :)

No, a taper is just a linear move between two axes, so G17/18/19 don't come into play. This is tough to explain in words, isn't it? Hmm.

Let's say you had a bowl shape to mill and you wanted to hand program it. If you machined the bowl shape in the X direction, you would need to program all of your G2/G3 moves in G18, however if you wanted to do a zillion tiny linear moves, it wouldn't matter what arc plane you're in because linear moves are not affected.

Also for visualizing this lathe business, I think I see where you're getting confused: For mill work in G17, your arc plane is parellel to the table, so picture laying a big piece of cardboard on the table, put a pencil in the spindle and draw a circle with it. Now for the lathe stuff, rotate the cardboard up and towards you so you're looking at the broad side of it, with the pencil still in the spindle. Now the cardboard represents G18. The cardboard is where all arcs will happen. If you run the same exact program as before except with G18 active, the pencil would draw the exact same circle on the now vertical cardboard. I hope I'm not confusing things even further! :)

And ofcourse the easiest way to figure it out is to go mess around with it. Program a 10" or so G2 in G18 and watch what happens.

Geof, the reason I asked about setting work offsets is because it takes a long time (for me) to calculate each individual work offset relative to G54, and then hand type it in, plus the obvious chance for mistakes. I was looking for a way to automate this somewhat.

..... This is tough to explain in words, isn't it? Hmm. ....

....Geof, the reason I asked about setting work offsets is because it takes a long time (for me) to calculate each individual work offset relative to G54, and then hand type it in, plus the obvious chance for mistakes. I was looking for a way to automate this somewhat.

It is tough to explain in words but you did a better job than me I think; my problem is people can't see me waving my arms around to make things clearer. :)

Regarding automating your work offsets? Here is the procedure I think I would use if I was doing turning on the mill as we are discussing. This is sort of based on how I do offsets for gang tooling on my TL; on the lathe I rarely use work offsets so my tool offsets are taken from machine zero. The procedure is to have a piece of stock in the chuck, turn a diameter, any diameter, and without moving the X axis enter the X coordinate in the X entry for the tool offset (on a Haas this is a single key push). Now measure the diameter and add the negative of this to the X entry (again on a Haas this is a single key push). The result of these operations is that the tool tip is at X zero at the centerline of the spindle. Now take a face cut across the stock and enter this in the Z entry (again one key push for me). Now Z zero is at the face of the part. For the other tools repeat the turn diameter, etc sequences, but only touch off on the Z face do not take more off.

Moving to the mill again have a piece of stock in the chuck; choose a tool, turn a diameter and enter the X coordinate into the X column for the chosen work zero. Vern for you this would be push ZERO PART SET with the cursor highlighting the X space for the chosen work zero. Measure the diameter and add the negative of half this to the X value. Vern this would be type -(half the diameter) and push write. This puts the tool tip at the spindle centerline.
Now face off the end of the stock and enter the Z coordinate into the Z column for the work zero. Choose another tool and work offset and repeat everything for this tool.

I haven't mentioned Y so far but off course if the tools are not in line along the X axis it will be necessary to adjust each tool so that it is cutting on center and enter that Y coordinate in the Y column. Then whenever you move to a different tool in the program you would have a Y0.0 command to center that tool.

And I have no idea if this makes things more or less clear; it seems perfectly lucid to me but I have the advantage of a nice bottle of McEwans Scotch ale and a big glass of wine to help my understanding.

The fog is clearing, my terminology was poorly chosen for the result of G18 but I had the plane designation right and Matt's cardboard made it stick. I'm getting a good handle on Geof's suggested procedure for setting work offsets because it's very similar to what I do now. I am curious about the second and subsequent tools.

While you could continue to take small cuts to set X for each succeeding tool and do the math to find the spindle center-line I would think you would only want to bring your faced off surface from the first tool offset procedure into contact with all the subsequent tools for the succeeding Z offsets? If I'm correct here some of these could be daunting, like the point of a drill. I would think a boring tool could also present some interesting problems. I can see where a lot of on the machine tweaking could be necessary here.

Once again, my lack of knowledge about CNC lathe operations is probably getting in the way.

Both Matt and I have the luxury of a Renishaw tool setter and probe so we would naturally want to involve it in as much of this as possible. :)

Vern

...... I am curious about the second and subsequent tools.

While you could continue to take small cuts to set X for each succeeding tool and do the math to find the spindle center-line I would think you would only want to bring your faced off surface from the first tool offset procedure into contact with all the subsequent tools for the succeeding Z offsets?...

.. If I'm correct here some of these could be daunting, like the point of a drill. I would think a boring tool could also present some interesting problems....

I can see where a lot of on the machine tweaking could be necessary here.

Vern

Yes take cuts for X but just touch for Z, this is what I meant by touch off do not take more off.

For touching off my 'probe' is a piece of printer paper held between the tool and the part and jiggled until it is just gripped. Paper is remarkably constant thickness at about 0.003". For drills you don't need to worry further than that, how often is a drill depth critical to less than 0.01" or more? For a boring tool you can just enter the correction based on the paper thickness. Aternatively mark up the end of the stock with felt pen and with the spindle turning slowly advance on the slowest jog (0.0001) until you scrape of the felt pen ink and see a shinier ring. X for boring tool of course needs a hole bored and measured.

For the boring bars, what I do to set X is to spin the spindle backwards and then do exactly like the OD tools except on the opposite side of the work. No need to drill and bore a hole in a setup part that way. Once you do M3 S2000 or whatever in MDI, that RPM stays active even after a reset (if I remember correctly), so all you have to do is hit the CW or CCW buttons and the spindle goes to the last commanded RPM.

Now about the probes. If you use the table probe to set the H offset of the material, then you MUST use the spindle probe to set all the Z heights of the tools. Just like in milling, if you use the table probe to set the H offset of an endmill, then run over and touch the endmill to the top of the work and hit 'part zero offset', it will NOT work. I have no idea why this is, but I found out the hard way.

and Matt's cardboard made it stick. You have no idea how proud of myself I am right now. :D :p

Matt,

It's always nice to make folks feel good. :)

I know this has to be simplistic reasoning but let me try it anyhow. You have a plate with 2 boring bars, two drill chucks, and 3 turning tools solidly mounted. You have a reference hole in the plate to use as your initial G whatever. I'm sure you know where the center line of the drill chucks and boring bars are in relation to your reference hole. You also must know where and cutting edge of the turning tools are in relation to the reference hole. I would think the only way any of these would change would be from replacing any of the 7 tools, and it looks like you are using all insert tooling so that would be minimal.

With all this known information, and assuming one used Goef's method of working all your offsets from the spindle center line why can't all the X and Y offsets be entered by mathematical computation with all these known points? If your planning on turning something from a 1" diameter piece of work to a finish diameter of .75 can't you offset the known turning tool end point by .5 and start moving in from there? I imagine you also know all the Z height measurements from the plate (excepting the drills length) so I guess if my reasoning is correct you could also set the tool length offsets from these known values as well.

Please keep in mind that I've never programmed a lathe so as I said this is probably simplistic.

As a side note, I've watched your video several times and noticed the location of the boring bars as they relate to the drill chucks. If you went to the ER 32 collet chuck as suggested by Goef you might have a problem hitting a tool ( drill ) in one of the chucks with the bottom of the spindle.

Vern

.....I know this has to be simplistic reasoning but let me try it anyhow. You have a plate with 2 boring bars, two drill chucks, and 3 turning tools solidly mounted. You have a reference hole in the plate to use as your initial G whatever.....Vern

Yes, simplistic, but correct. As an aside, have you ever noticed how human beings seem to come up with the complicated first, before they get smart and simple. :)

If I interpret your simplicity correctly you are considering a setup her all the tools have a know relationship to the reference hole. In this situation all you enter into the machine are the coordinates for the work zero that is placed at the reference hole. All the relationships between the individual tools and the reference hole are given in G52 commands that are included in your part programs. And I made that bold because it is what makes your idea simple and effective; and easy to set up because you only have to determine a single location each time.

I hope I am not sticking my neck out on this but I think I have it correct.

But have we introduced you to G52? I think I mentioned it in a different thread, have I mentioned it in this one?. You have your reading cut out for the next couple of evenings; also do some searching on the zone, G52 has been discussed at length.

I've been following carefully for months your references to G52 and Gar's gusher of macro recommendations. :)

I certainly don't understand 90% of it but can see that not figuring it out and using it effectively is locking myself to yesterday. The really sad part is; I will probably become a semi competent hand programmer despite my knee jerk dependency on my CAM program.
:D:D

Another item in the millathe discussion I have to deal with is the necessity of multiple work offsets without a single tool change (I hope).

Vern

I've been following carefully for months your references to G52 and Gar's gusher of macro recommendations. :)....Vern

If gar reads this I hope he is not too, too, offended; (sotto voce) for the moment ignore what he says; if I try hard I can follow a lot of it but don't worry if it flys over your head. :D

sotto voce? from the land of the Romans, I thought your recent visit to the Germanic canal/river system spoke of a different heritage, like Smith. :)

sotto voce? from the land of the Romans, I thought your recent visit to the Germanic canal/river system spoke of a different heritage, like Smith. :)

Heritage? Anglo Saxon, probably. Anyway the river system you must be referring to spends more of its time in non-Germanic regions, doesn't it? I would have to refer to Google Earth to confirm, but the system I have that loaded onto is down at the present.

The reference is very dependent on the time frame. If my fading memory is correct the Romans considered all area north of the Alps the preserves of the Goths, Visigoths, Celts, and various Mongol Hordes. Most of these aggressive fellows who resided on the European continent were considered Germanic tribes.

Please don't consider this an attempt to cast dispersions on your heritage which seems to be Celtic or Norse by your description. My Mothers side (McCracken) is very Scott / Irish I'm told, who shared the British Isles with your ancestors.

It will be interesting to see what the moderators think about the digressions of this thread tomorrow morning. :D

I did a quick check to make sure this was your thread so if you are aiding and abetting in a hijack that is okay, I think. :D

Don't worry about casting aspersions on heritage; I do not really have much idea about my own but it is probably Germanic.

think rather than North of the Alps it was North of the Danube; that acted as the most effective barrier. There were several Roman settlements on the Danube; well the South side that is.

And if your heritage is Scottish/Irish you should find some books about recent genetic studies. I read one recently which looked at the genetic heritage of the MacDonalds that came to the conclusion that the founder of the clan was actually Scandinavian, from Viking times, not Scottish.

So you might be the Norseman, not me.:D

And don't worry too much about moderators, if you started the thread surely it can go in your direction?

And if your heritage is Scottish/Irish you should find some books about recent genetic studies. I read one recently which looked at the genetic heritage of the MacDonalds that came to the conclusion that the founder of the clan was actually Scandinavian, from Viking times, not Scottish.


Just an aside to the digression. If either of you are interested check out PREBBLE, JOHN The Lion in the North. One thousend years of Scotland's history, 1973. It goes into depth about the Norse influence in Scotch history.

On topic. How well could a threading cycle be performed with this kind of setup using a lathe ID threading tool? I'm sitting here twirling my fingers and thinking that with a plunge in Z with the appropriate speed/feed rate could produce either hand thread depending on the spindle rotation, using a left and right hand tool. Or one tool and make a Z-/Z+ move as appropriate. Could spindle orientation be added to this to to allow for a spring/finish pass too?

Just an aside to the digression. If either of you are interested check out PREBBLE, JOHN The Lion in the North. One thousend years of Scotland's history, 1973. It goes into depth about the Norse influence in Scotch history.

On topic. How well could a threading cycle be performed with this kind of setup using a lathe ID threading tool? I'm sitting here twirling my fingers and thinking...

I will check the book, and on that topic have you read the called something like; "How Scotland Came To Rule The World".

On the thread topic: Twirling fingers is okay, I do that a lot, but thinking? Getting into risky territory here, might hurt my brain. :D

I mentioned it a few posts back just as an aside and then did think a bit and convinced myself it would not be possible. For lathe threading the spindle rotation and Z axis movement have to be synchronized with respect to speed; rpm to ipm. But there is additional synchronization between the X axis, the spindle orientation and the Z axis so that the tool enters and leaves the cut at the same point. You probably could code the moves for a single threading pass that may come out quite good because the rpm and feed rate are quite constant, but would you ever get back to the same start point for a second pass. Unlikely to the point of being impossible I think.

Tapping would be possible but for external threads you would need a die-head; of which, I have one sitting on a shelf somewhere left over from my pre-CNC days.

I will check the book, and on that topic have you read the called something like; "How Scotland Came To Rule The World".

On the thread topic: Twirling fingers is okay, I do that a lot, but thinking? Getting into risky territory here, might hurt my brain. :D

I mentioned it a few posts back just as an aside and then did think a bit and convinced myself it would not be possible. For lathe threading the spindle rotation and Z axis movement have to be synchronized with respect to speed; rpm to ipm. But there is additional synchronization between the X axis, the spindle orientation and the Z axis so that the tool enters and leaves the cut at the same point. You probably could code the moves for a single threading pass that may come out quite good because the rpm and feed rate are quite constant, but would you ever get back to the same start point for a second pass. Unlikely to the point of being impossible I think.

Tapping would be possible but for external threads you would need a die-head; of which, I have one sitting on a shelf somewhere left over from my pre-CNC days.

I'll check it out. As a 3rd generation removed Scot myself I enjoy reading how most great statesmen and inventors in western society have been Scots or descended from Scots, little racial pride showing ;)

I twirl my fingers so I don't hurt my brain! It always tickled my instructor in school, even more so my wife when I was doing homework. My Mickey Mouse (Sorcerer's Apprentice) cutter comp technique she called it. :)

I missed the threading post from earlier in the thread, sorry. Will go back and read it. Of course a lot of parts could be later thread milled with a different setup as a secondary OP I guess. Our shop has a pretty good lathe but as an exercise in thinking outside of the my norms I find this a pretty interesting thread and it is giving me ideas, thanks to you for that Vern. Think about several blanks in tool holders in the ATC and making this all a series of subs like you've (Geof) posted in the past. It could allow someone to make some parts or assemblies without having to sub the lathe work out.

I'll check it out. As a 3rd generation removed Scot myself I enjoy reading how most great statesmen and inventors in western society have been Scots or descended from Scots, little racial pride showing ;) ....

That is exactly what the book is about but I did get the title wrong. It starts somewhat before the Act of Union back in the 1700s and then follows through all the developments made by people who where either Scottish or educated in Scottish universities or other universities founded by Scotsmen.

I am all in favor about thinking outside the norm; I wondered about starting a thread "What is the most 'outside the box' setup or machine use you have done".

I am all in favor about thinking outside the norm; I wondered about starting a thread "What is the most 'outside the box' setup or machine use you have done".

I might have to refrain from posting to that one. I couldn't stand to have you all laughing at me! :p
What was is Clemons said, better to be thought a fool than to open one's mouth and remove all doubt ;)

Vern have you given much thought to the first "millathe" project you plan to program for? A plumb bob might be an idea. It would cover the radius and tapers you were asking about earlier. Just a thought.

I might have to refrain from posting to that one. I couldn't stand to have you all laughing at me! :p
What was is Clemons said, better to be thought a fool than to open one's mouth and remove all doubt ;)....

It is unlikely I will ever laugh at anyone because they tried a crazy idea and it worked; I may laugh with them when they try a crazy idea and it doesn't work; my response to people who are to stodgy to try crazy ideas is not to laugh but just shake my head.

The plumb bob is a good idea whether you are using a millasalathe or using a lathe; and the finished item is useful.

Think about several blanks in tool holders in the ATC and making this all a series of subs like you've (Geof) posted in the past. It could allow someone to make some parts or assemblies without having to sub the lathe work out.[/quote]

Dear Lord, now I have to figure out subroutines as well. :confused: I'm not sure all this is within my grasp. :)

There are a specific and very simple pair of aluminum flange bushings I had in mind when Matt's video caught my eye. It took me almost 7 hours to make them on my El Cheapo manual lathe and bored me to death. I agree the plumb bob is a good test subject; however, at this point I'm trying to learn enough hand coding and how G12 works for offsets that avoiding a crash is priority number one.

The Haas teck showed up today and installed my Renishaw system so learning how to use that is currently on the front burner. In the short demo he did for me I can see it will save me hours and hours, which I can devote to hand coding, g12, sub routines, etc. etc. :D

To digress to ancestors, history has given the Norseman or Vikings a bad rap. These guys were amazing. Not only were they fearless seafarers but they traveled incredible distances to trade. Many archaeologists have found their artifacts on the shore of the Black Sea. They are credited with using the river systems of interior Russia and Belarus to get there. Only problem is several areas required portages of up to 100 miles between river systems. Can you imagine carrying river boats full of goods to trade with the Persians over land for 100 miles. These were some heavy duty fellows

Vern

Geez, don't any of you guys work during the day?! :)

Vern, check out the attached program. It is incredibly simple to do subs...if I can, then you can, trust me on that. The attached program is a whole-machine warmup. My mill can sit for up to two weeks at a time, so this gives me some piece of mind.

As far as threading goes, I've yet to try it but I'm tempted to say that thread milling would produce low enough forces that a drill chuck could be employed to hold the thread mill and bingo, you can thread ID and OD. I would think that thread mill canned cycles or CAM outputs would be exactly the same as when using your mill as a (ghasp!!) mill.

Matt,

Thanks for the warm up program with the two (I think) subroutines. If you tell me that M97 followed by P1000 is calling a subroutine starting on line number N1000, then I think I've got it.

Assuming we use G12 to move from tool station to tool station would subroutines be used to simple rerun the entire program after the tool change brings in a fresh blank?

I've been giving the idea of running multiple blanks with tool changes some thought and I'm a little concerned about finished pieces laying around at places we don't want them. Maybe we need to put a small whisk broom in one of the collet holders and call it every couple of cycles to sweep the table free of any finished parts that didn't fall where intended? :)

Do I work during the day? Unfortunately yes, I was supposed to be retiring but things got busy. Most of my time is spent doing prototypes and tooling and sometimes my machine has a cycle time of 10 minutes to over an hour so I amuse myself here.

Vern; you have subroutines straight; when you are using multiple work zeros it works out that the main body of your program is often just the work zero selection followed by a subroutine call and your part processing program is all in the subroutine(s).

It gets a bit hairy sometimes keeping things straight.

Matt,

Thanks for the warm up program with the two (I think) subroutines. If you tell me that M97 followed by P1000 is calling a subroutine starting on line number N1000, then I think I've got it. That's exactly it. See? Easy.

Assuming we use G12 to move from tool station to tool station would subroutines be used to simple rerun the entire program after the tool change brings in a fresh blank?
Anyway you do your work offsets, I think using local subs would be the best way to do what you're talking about. Lots less programming that way. Well, by a factor of however many blanks you intend on loading in the machine.

Whisk broom? Good thought, but I can assure you that your finished parts will go wherever you don't want them to, and it won't be very consistent. Most of mine fell into the coolant trough (where I had cardboard to cusion the fall), but sometimes they would shoot past all that and end up in the damn chip auger. One of 'em is in my chip barrel right now, but I sure can't find it.

.... but I can assure you that your finished parts will go wherever you don't want them to,...

But at least gravity is on your side pulling them away from the spinning thing. On a lathe when they happen to fall between a chuck jaw and and adjacent tool in the turret there is an almighty bang, sometimes followed by a big bill to pay for getting the turret re-aligned.

Geez, don't any of you guys work during the day?! :)


45 min cycle times on both of our mills with about 1.5 minutes to load both, and they finish right behind each other :) Lots of pretty 316 chips but the coolant flushes them clear so until it is time to load, or adjust a geometry offset or find/replace a T0n;H0n;D0n it is pretty much just like watching paint dry. Shame I have nothing going for the lathe right now, usually that keeps me out of the office and on the floor. :p

Vern, subs aren't hard to learn, you just need to keep a few things in mind. HuFlungDung and Geof both helped me tune my first hand coded one here the other month. Original program was pages of typed code and went down to about 60 blocks all together if I remember correctly. Subs are powerful tools. Example of it is 1 million holes in a grid pattern. A program for a spot drill and sized drill can be written in under 30 blocks, well worth learning as you go along with learning to hand code a program. Check out the replies here : They not only helped me with the logical progression of the code but also lots of good advice on keep things consistent to avoid mistakes that go BANG.

Scott

.... Subs are powerful tools. Example of it is 1 million holes in a grid pattern. A program for a spot drill and sized drill can be written in under 30 blocks, well worth learning as you go along with learning to hand code a program....Scott

Just to stick poke, because I am pretty sure you won't go off the deep end :)I think I have one that can do it in 28 lines and that includes some comments.:stickpoke

I am thinking about a bragging thread showing a program with dozens of work zeroes and subs just for fun. Should I do it?

Don't get shy on us now Geof, go for it. Besides I need the free training. :)

Just to stick poke, because I am pretty sure you won't go off the deep end :)I think I have one that can do it in 28 lines and that includes some comments.:stickpoke

I am thinking about a bragging thread showing a program with dozens of work zeroes and subs just for fun. Should I do it?

I've looked again, I'm not seeing where I could shave off but one block, an optional stop. Can I write my safety line (G20 G40 G49 G80 for me) and my T01 M06 on the same line? I was taught to separate them for obvious reasons but I don't see where they would conflict so that would remove another line leaving room for one comment and keep it at 28. Past that I think I'm stuck.

As to the other thread idea, it would be educational for me to see how you keep track of the different work offsets. When using more than two I always draw up a quick setup sheet with major features and dimensions to keep my part oriented correctly, but unless I'm subing out to multiple vices/fixtures it gets a little confusing. If you want to break it up into sections to make it easy to follow I think it would be educational. I know Vern is tied up with his new Renishaw probe right now, lucky guy, but it would help him with his lathe mill idea too down the road.

Vern is it true those probes can be used to compensate for misalignments, within limits, in X,Y and Z? The Mazak tech was telling me that on their mills it would, I'm wondering if it works the same on a Haas.

Scott

.....leaving room for one comment and keep it at 28. Past that I think I'm stuck......

....As to the other thread idea, it would be educational for me to see how you keep track of the different work offsets.....Scott

If you roll lines together that it is sometimes best to keep separate I think you can get shorter but that is kinda cheating.:)

Regarding keeping track of offsets: I type up an initial description of what I am going to do, and while designing the tooling and writing the program I keep going back to this description and updating it.

I will put up my thread with pictures and a copy of the program later this evening.

Scott,

The probe/tool setter equipment is very impressive. I've only had a few hours of play time so I'm just scratching the surface. The guys who will be helpful here are Matt and Cory.

Like you, I have heard that the system will correct for a misaligned part or fixture plate. All I've used to date are the Haas Visual Quick Code templates that come with the package. I didn't see where any of these will do it but I've heard the Renishaw software will. One of the Haas options that are included with the Renishaw package is rotation and scaling. If I understand the rotation feature correctly I would think that option would allow the Renishaw to trigger the Haas rotation option which I would think is necessary to skew any of the three planes. Don't mean to sound like I know what I'm talking about because I don't. :)

Vern

Scott,

Did a little research last night. I've attached pages from the Renishaw manual that cover the area you were questioning. As you will quickly note this is not intuitive stuff. As a matter of fact it looks just like the code GAR posts now and then. :)

As I said, the Haas package includes many pre-written macro programs that locate holes, sides, bottoms, etc. These are obviously supplied to find work offsets. I could not find any measuring programs per say in the Haas VQC programs. However; it doesn't take a lot of effort to turn the Haas location specific programs into measuring devices.

Locate the back of something and the Haas program puts the number into the Y column of the offset page (you select the offset #) Locate the front of the something give it a different offset number. Go to the offset register and subtract one from the other and You've got the dimension. Sizing a hole? Locate the center, locate the side and do the math.

The trick here will be learning how to write macros as described in the attached pages to do all these measuring functions. Looks like fun. :)

I made several attempts to up load the zip. for the portion of the manual. It's well within the size limitations. Not complaining considering what I pay to be on this forum. If it's not there I'll try later. It looks like Goef had similar problems with his most recent thread.

.... It looks like Goef had similar problems with his most recent thread.

Are you referring to the absence of a program when I said it was uploaded?

I forgot :) it is there now.

Your comment about probing and compensating for mis-alignment of a fixture plate needs the option Rotation and Scaling; does that come in the probe package. I seem to recall quite a while back someone posted on this topic and they must have had a macro because they simply probed in two locations and could then read the correct angular value into the command setting up the Rotation.

But a Real Machinist doesn't have mis-aligned fixture plates. :D

Yes, If I can get the site to accept my up load the macro and function is described. Rotation and scaling come with the Renishaw probe package and the macro automatically triggers it to correct for an Wimp Machinist's mis-aligned fixtures. I'm getting that Harley biker image again. :) :)

I think I have the up load now.

..... I'm getting that Harley biker image again. :) :)

Never Harleys; started on a little BSA, another little BSA, a Matchless (have you ever heard of them?), then a BSA 650 Road Rocket. Gave it all up when I started a family and piled off my Yamaha in front of my daughter.

Regarding mis-alignment...this brings out one of the neatest aspects to CNC, at least from my perspective as a long time manual machinist, you can correct just by pushing a few buttons and entering a few numbers; that is so convenient when you are just slapping something on the table quickly, simply not possible on a manual machine.

If you go back a couple of posts you will find the pages from the Renishaw manual that cover the current subject. If I have the era you are referring to correct the hot item in my area of the USA was Thiumph Trophy Birds and Bonnivilles. I had two of the former. I never had a bad spill on a bike but I took about 6 pounds of meat off sliding to a stop on asphalt after going upside down in a go kart, twice! :D

Yes, If I can get the site to accept my up load the macro and function is described. Rotation and scaling come with the Renishaw probe package and the macro automatically triggers it to correct for an Wimp Machinist's mis-aligned fixtures. I'm getting that Harley biker image again. :) :)

I think I have the up load now.

What kind of tickled me was the idea of correcting in the z plane for flatness tolerances. After rebuilding our Kurt vises, using their tech support and reading a couple of in depth threads on this site I still have a problem with thin stock lifting .0008 to .0012. The probe could help with that I'd think. We don't usually need more precise vises than we have, but every now and again... You get the idea.

......I still have a problem with thin stock lifting .0008 to .0012. .....

Are you using the little O-rings that go under the leading edge of the moving jaw which hold the jaw up slightly when it is not under pressure but which compress and allow the jaw to move down firm against the base when it is tightened?

Are you using the little O-rings that go under the leading edge of the moving jaw which hold the jaw up slightly when it is not under pressure but which compress and allow the jaw to move down firm against the base when it is tightened?

It was one of the first repairs I made when I removed the movable jaws to clean under them. I later replaced the thrush washers etc that come in the kit from Kurt as well. With as many tool marks, from drills to fly cutters, and as much crud and flattened chips as I removed from behind the removable jaws when I started I'd say they where probably used pretty hard with little maintenance. Our parallel sets are pretty cheap enco specials, but I surface ground all of them in groups so they are true, flatness and height, but were less than a thousandth out to start with so it might have helped a little but not that much. It isn't often that I make parts that it exceeds the tolerance, but all the same it isn't right so it aggravates me.

The migration of this thread is a case study in deductive reasoning. Since Kurt vises and their proper use has come up I would like some more advise. :) The instructions that came with my 688's referred to use of the little "O" rings as not recommended for step jaws. I use some of both, probably favoring parallels in straight jaws. In the dual use situation are you better off having them in or not in?

Another item is the thin sheet metal chip guards supplied. I'm certain they would work beautifully but the amount of the opening in the jaws affects the length you need for your chip guard. If you set up and run the same part all day I can see where they would be handy, other wise they never seem to fit the opening of the moment. Forgetting to take one out that's set up for a wide opening will not do it much good when the table heads for the back of the machine.

With regards to the little O-rings that are supposed to allow the vise to clamp the part down onto parallels I never use them because it is my expectation that chips will almost instantly get under the moving jaw and negate their function. If it is necessary to hold something down firmly against parallels I use a block of UHMW polyethylene on the part and a piece of material in a toolholder to push it down gently with the spindle. This of course is impractical on a production basis but quite okay for one offs.

Rgerading the chip guards I find they are very useful to cut up for shim stock; pretty close to totally useless on the vise :). And I cannot recall ever having a vise screw jam because chips got carried into it.

I see Florida's charms did not hold you for long. :) Thanks for the info. I've never used either but wanted to be sure I wasn't missing something.

Rgerading the chip guards I find they are very useful to cut up for shim stock; pretty close to totally useless on the vise :). And I cannot recall ever having a vise screw jam because chips got carried into it.

I can believe that since I had to use a screw driver and shop vac to clean out a couple of the ones we have. If nothing else I'd say the vises where well greased :)

I was able to tolerate the Florida heat; which wasn't too difficult since I was either inside an air-conditioned exhibit hall during the day or an air-conditioned bar in the evenings. :)

I think the reason our vises have not had jamming problems is they are used almost exclusively on alumininum, i.e. biggish chips, with flood coolant, and we never grease the vise screw.

i wasn't sure where to post but I'm a newbie. well 49. anyway Ive been out of work for over a year now and i just started school for cnc/cad and I'm like in aaaaaaa! Ive been setting up thread rollers most my life so i know a lil about the (..........) DOTS lol but its the G Code and trying to remember everything.

so what I'm trying to forget everything that I think I new and everything that I thought I new and come to find out I know nothing lmao! so HELP I can see light at the end of the tunnel so I'm TRUDGING along. Oh I'm not book smart and I'm a recovered alcoholic with ADD/ADHD. So having Fear of going back to school I had my hole life and I had to over come that Fear and here I am.

I just thought I would come right out and be Honest with you all.

Carlon

Ps. Yes I do use spell chack can you tell?

....I'm like in aaaaaaa!.... its the G Code and trying to remember everything.

so what I'm trying to forget everything that I think I new and everything that I thought I new and come to find out I know nothing lmao!....

My response to your last comment first: Wrong approach...add CNC onto what you already know. For an experienced machinist/toolsetter/whatever, CNC is an enhancement to their skills.

Response to first comment: Don't try to remember, there are too many codes that have no intutive interpretation it is almost impossible to remember them unless you are using them every day.

Make your self a pair of 'mirror image' lists: I say mirror image because one list has the G code down the left side in numerical order, which is how they are normally presented; G00, Rapid move, G01 straight line interpolated move, G02 clockwise circular interpolated move, etc. The other lis is in alphabetical order; Clockwise circular interpolated move G02, Rapid move G00, etc.

This way if you remember a code you can quickly check whether it does what you are wanting. Alternatively if you know what you want the machine to do, for instance spot drill for starting a hole, you look it up in your list; Spot Drill hole G82.

I was thinking, and I had not even had my morning coffee! The mill, of course, does not have G76 or G92 threading cycles which both synchronize X and Z to the spindle rotation; X to a specific point in the rotation, and Z to the rate of rotation. But it does have one canned cycle that it may be possible to use to 'fake' G92, and that is G84 when it is used with Repeat Rigid Tapping turned on, aka Peck Tapping, because G84 will repeat at different X locations. There is one problem, however, and that is that G84 reverses out of the hole, but maybe this will work:

Mount a tap so that one cutting edge is on center to the work piece in the spindle.

Set the X starting position in the G84 so that the OD of the workpiece lines up with the OD of the tap; set Z as the thread length (depth) as normal.

On the lines following the starting line for the G84 move the tap in toward the workpiece in small steps just like normal lathe OD threading. Just as if you were Rigid tapping a lot of holes.

The reason for using a tap is that there will be a lot of rubbing during the reversing so a carbide threading insert would probably chip; taps can handle being reversed.

This works when I visualize it in my mind but with one thing I haven't quite got straight: Would a lefthand tap be needed for cutting a righthand thread this way? Even though I have now drunk the coffee I haven't sorted that out. Other than that I think it could work in soft metals like brass or aluminum.

To make normal right hand OD threads you would need to use a right hand tap.
But you would need to cut the end off and re grind the cutting edge on the other side of the flute as if it were a left hand tap.

A left hand tap would have the wrong helix angle.


Edit:

To hold the tap better you could.
Tap a hole near the edge of a block of steel.
Then mill some off that edge so the when the tap is in the threaded hole one cutting flute is sticking out.
Band saw a slot and add some clamping bolt holes so you can hold the tap solid.

May want to hold the tap at a small angle, 1/4 degree or so, so that it does not rub along it's entire length. But not enough to noticeably affect the thread being cut.

Nice to find someone take a slightly crazy idea and give suggestions for making it work better. I had hoped to avoid re-grinding a cutting edge because that would be a bit finicky without a good grinder. The slight angular adjustment certainly would help.

The clamping suggestion would need a four flute tap to get the best effect possibly.

Come on Vern give it a try. :)

EDIT: I guess we had better watch out for the "USE THE CORRECT TOOL FOR THE JOB" sticklers. Although one could argue given the constraints of the situation this is the correct tool.

EDIT: I guess we had better watch out for the "USE THE CORRECT TOOL FOR THE JOB" sticklers. Although one could argue given the constraints of the situation this is the correct tool.

Slam me up side the head...

Inserts for those self opening die heads used on Swiss and turret lathes. They have nice flat sides to clamp on.

Or you could cut up a round die.

For small stuff you could just use the die and cut the thread in one shot.

A few posts up I mentioned using the regular self opening dieheads, although Z space could be an issue.

Cutting up a die-nut or a split hand die would work and give the correct cutting edge and helix. Using the inserts from a die-head I am dubious about; I have used these and they chip at the leading edge very readily, I think they may not handle the reversing.

This is probably way off base since I've never used one but how about using a thread milling tool? Wouldn't that give you the cutting edge on the right side plus solve the rubbing issue? Of course it could be skewed a bit as well but that sounds like a huge PITA when making the tool plate.

If we are employing the peck tapping feature and it solves the synchronization issues previously described, I don't see why we don't use a simple lathe threading tool and do away with all the angular and rubbing issues. Remember, I have a penchant for simplistic thinking. :)

Vern

....I don't see why we don't use a simple lathe threading tool and do away with all the angular and rubbing issues. Remember, I have a penchant for simplistic thinking. :)

Vern

We cannot do away with the rubbing when the spindle reverses.

When threading on the lathe the tool withdraws from the cut on X and then retracts on Z back to the Z coordinate at the beginning of the thread; the spindle keeps on rotating. It then moves in on X and synchronizes the Z movement with the spindle rotation for the next pass along the thread; this requires coordination between the spindle position for the start of the X motion and the spindle rpm for the Z motion.

On the mill there is no coordination between the X motion and the spindle rotation; only Z is synchronized and with Rigid tapping it is synchronized both for forward and reverse rotation to withdraw a rigidly held tap and then re-enter the hole with the thread aligned. The rubbing I mention occurs when the spindle reverses and withdraws upwards, it cannot be avoided.

This why I do not think a single point lathe threading tool would work; I expect it would chip, particularly if it is carbide. A carbide thread mill I think may also be prone to chip.

The point is, of course, that the way to do it is experiment.

Ah, now I see, I guess I'll have to buy a CNC lathe and do some programming so I can keep up with you guys. How about mashing on the E stop every time the spindle gets to the bottom? :)

In a more serious vane, assuming we machine a groove in the part where our threads will end and start the threading plunge far enough above the threading tool that our spindle motor and Z axis servo have time to stabilize, how about this. The Haas mills have spindle orientation. Rather then using G84 could the threading code be created by hand (how about that Goef) orienting the spindle at the beginning of each pass, then using the necessary speed and feed normally used in rigid tapping for the down stroke. Stop, back off retract to where you started in Z and repeat with the spindle center line moved in the amount of depth you want to use for the next cut.

I hope Matt is watching because He's got the whole set up ready to go and could try this stuff tomorrow, assuming he can forget about little formalities like making a living and such. :D

.... The Haas mills have spindle orientation. Rather then using G84 could the threading code be created by hand (how about that Goef) orienting the spindle at the beginning of each pass,....

Check what the spindle does when you give it a M19 Psomething command. It does not move just from where it is to the commanded orientation in the shortest manner it will sometimes do almost a full circle. But then when it is oriented you cannot start the spindle and the axes simultaneously; M codes are processed after all the G codes in a command block.

For the moment, I'm out of airspeed, altitude, and ideas. :)

I am a bit late, but better late than never.

This was Vern's Thread starter post: Six or so months ago there was a thread on this forum featuring a fellow who set up various lathe tools and drill chucks on a plate mounted in vises on his mill table. He put bar stock into the spindle and used the mill to perform limited lathe functions. I have not been successful finding it with the search function, does anyone remember it?


I think operative time span was the 'or so', not the six months. I was mooching around and found some threads starting back in 2006.

http://www.cnczone.com/forums/showthread.php?t=25408

http://www.cnczone.com/forums/showthread.php?t=34697

And the link below shows the same video that Abdre' B linked ib Post #3 but this one shows who was doing it; a member called metalbyter

YouTube - Taig mill turning bushings

EDIT:

To see the complete thing you need to put the 'http://www.' in front of the website address below and copy/paste it into the address bar. Then you will also have access to some other videos.

youtube.com/watch?v=wbfXXeiSHsw

Goef,

I appreciate your rummaging around in the archives to find these. I just got the last of the necessary tooling to set up a tool plate. One of this weeks projects is to make the plate and figure out the necessary programming. I think I have a fighting chance thanks to the material posted in this thread. :)

The Haas folks are coming tomorrow to provide the training for my Renishaw package. Probably just enough knowledge to be really dangerous. :D

Goef,

I appreciate your rummaging around in the archives to find these. ......

Except I was rummaging looking for something different, which I didn't find, and now cannot remember what it was.

I find search engines are distracting; you put in the terms that you hope will bring up your subject, they don't but you see something interesting in the list and pursue that, then a few minutes later your mind is a blank regarding the original search.

If you're having memory problems now wait until you enter your "Golden Years". :D At my age this is a daily occurrence.

Vern

If you're having memory problems now wait until you enter your "Golden Years". :D At my age this is a daily occurrence.

Vern

I thought I was in my so-called Golden Years; I must be, the memory thing happens hourly some days.

Da#n new fangled tooling :confused: I ordered one of the new (to me ) cut off holder, blade, and inserts for my Millathe tool plate. I'm trying to figure out how to secure the little insert into the blade. I can see on the insert that it has a small ridge that must want to be squeezed into place, locking it into the opening in the blade. They sent along a tool that looks like a single flute Allen wrench. :)

My guess is that the tool is for popping the insert out of the blade because I can't see how it would function as a lever to spread the opening in the blade wide enough to lock in the insert. Is this a brute force move? Let the first application do the trick? While this may work where gravity is keeping it in the blade on a lathe application it's trying to make it fall out in this situation.

You fellows with real lathes will have to enlighten me.

Vern

Da#n new fangled tooling :confused: ...
Vern


Pictures! Pictures! Pictures!

Some parting tools need a tool to open the gap that the insert fits in, some have a little lever that is used to force the insert past a retaining ridge. Let us see some piccies and we may help; esp fails me at the moment:).

Your bid is my command, tomorrow. Let me think, my first wife took an esp seminar 35 years ago where the operative requirement was being able to sit in your chair and contemplate for two or three hours without a bathroom break. :) If you passed this test you could move up the the advanced class. She never made it, doubt if I would have either. I could never figure out the relevance of this; however, she always said she was smarter then I.

......sit in your chair and contemplate for two or three hours without a bathroom break. :)....

Bl**** h**l that is a wimp qualification:). I have done the British Airways flight from Vancouver to London without a bathroom break!! I admit I was not contemplating I was listening to my I-pod.

I've always contended their was a connection between bladder size and IQ. :D

I've attached a picture of the inscrutable cut off tool with the little box of inserts and what I presume to be a tool to pop the inserts out of the blade once one figures out how to get them in securely.

Vern

I've always contended their was a connection between bladder size and IQ. :D

I've attached a picture of the inscrutable cut off tool with the little box of inserts and what I presume to be a tool to pop the inserts out of the blade once one figures out how to get them in securely.

Vern

Direct or inverse?:D

Yes the little tool is to pop the insert out.

The getting them in securely is another matter. I think the manufacturer is under the impression that the cutting force will ram them in securely, because I cannot quite see banging them in with a hammer. I don't want to discourage you too much but you may not need the tool to get them out. We tried those parting tools and the inserts popped themselves out due to vibration in the machine and the shank alone makes a very poor parting tool. Two or three shanks mangled on the ends and a couple of boxes of inserts are still laying around somewhere.

Just give it a little tap with a plastic faced hammer to keep it in place until the first cut is made.

I have never used that brand but the Iscar cutoff blades I have used were never been a problem with holding the insert. At least until before they get tweaked by someone who should not have been using it.

Just give it a little tap with a plastic faced hammer to keep it in place until the first cut is made.

I have never used that brand but the Iscar cutoff blades I have used were never been a problem with holding the insert. At least until before they get tweaked by someone who should not have been using it.

We use Iscar now, DO-GRIP, they have a little lever thingy that pries the slot open so the insert slides in and then it springs shut onto the insert., they do hold securely. We tried the plastic hammer, and a little drift made out of aluminum against the bottom edge of the insert, but nothing we did ensured the inserts would stay in reliably.

I just wandered out and found the other ones; they are made by Mitsubishi not Tmax and the instructions do suggest using the plastic hammer...for all the good it did us.:)

I get a piece of aluminum or brass rod with a squared off end and give it a good square hit with a half pound hammer. Never busted one, never slips out, but don't try running the spindle the wrong way.:nono:
Run at about half the normal turning speed, solid feed, LOTS of compound.
Some times you need to peck to clear the curled up chips.:idea:
I've even made my own holder out of an old brazed on tip parting tool that had abused itself.:D Just used a hacksaw, file and a bit of patience.;)
Hit it hard. They are tougher than you think.:wave:
I use even big fat wide ones on intermittent cuts in 6' diameter multi vee pulleys, roughing out the grooves.
:cheers:

We use Iscar now, DO-GRIP, they have a little lever thingy that pries the slot open so the insert slides in and then it springs shut onto the insert., they do hold securely. We tried the plastic hammer, and a little drift made out of aluminum against the bottom edge of the insert, but nothing we did ensured the inserts would stay in reliably.

I just wandered out and found the other ones; they are made by Mitsubishi not Tmax and the instructions do suggest using the plastic hammer...for all the good it did us.:)

I use a brass drift for the same insert holder. A light rap with a small ballpean hammer to seat the cutting face into the brass and then a firm rap to seat it in the holder. Never had one pop out from plastics to 316 SS putting them in like that. I've since switched to the Iscar holder and inserts on the CNC lathe, but still use that same holder on the conventional lathe and seat them in the same manner.

Thanks for all the suggestions. I know carbide likes to chip so I was reluctant to beat it up too badly. No problem, we have brass and plenty of hammers.

"Direct or inverse?"

Now that's sticking your neck out!

Vern

............

"Direct or inverse?"

Now that's sticking your neck out!

Vern

Sometimes, somedays, I am pretty sure it is inverse. :D

Vern, that's the same exact parting tool I use and it will work fine. I don't know if these guys have actually had one fall out of the holder, but all I do is shove the insert in the blade by hand.

Matt,

You must have some formidable hands. I needed the brass and hammer method. Maybe mine is a little undersized. The plate is coming along, I don't have a good selection of boring tools so it's easier and cheaper for me to buy a couple of reamers.

Vern

Matt,

You must have some formidable hands. I needed the brass and hammer method. Maybe mine is a little undersized. The plate is coming along, I don't have a good selection of boring tools so it's easier and cheaper for me to buy a couple of reamers.

Vern

You are going to post us a video when all it said and done right?

....I don't have a good selection of boring tools so it's easier and cheaper for me to buy a couple of reamers.

Vern

Remember, if your drilled hole is off the reamer will follow it; reamers are not really a substitute for a boring tool but a means of attaining a final accuracy and finish quicker and easier than with a boring tool.

Remember, if your drilled hole is off the reamer will follow it; reamers are not really a substitute for a boring tool but a means of attaining a final accuracy and finish quicker and easier than with a boring tool.
To continue that thought, if you happen to have some resharpened or otherwise undersize endmills, you can drill, then 'ream' with an appropriate endmill to get your straightness and location back, then ream for size.

Thanks for the tips on keeping a hole straight and on size. I don't have a digital movie camera so you will have to take my work for the success or failure of this project.

I have been thinking about how imperative it is that a boring bar be dead vertical in this application. Obviously you would not want a drill chuck skewed a degree or two but the boring bar is basically a cutting point at a fixed location in space. I don't see how it matters what the orientation of the part ending with the cutting point is as long as it does not interfere with the side of the bore being cut.

I must be wrong from all the emphasis on a true hole to mount it in so please enlighten me.

Vern

... the boring bar is basically a cutting point at a fixed location in space. I don't see how it matters what the orientation of the part ending with the cutting point is as long as it does not interfere with the side of the bore being cut.

I must be wrong from all the emphasis on a true hole to mount it in so please enlighten me.

Vern

Correct, just avoid interference on the shank.

We sometimes use end mills with a corner radius as small boring bars and sometimes mount them slightly askew so that the cutting edge on the mill further back from the tip does not touch the bore.

I'm posting this hoping for constructive suggestions. It's simplistic and laborious in it's running documentation but that was the only way I could keep track of where I was and what I was trying to do. I've never programmed for a lathe so this can't be very "lathe" sounding. I've never hand coded for a mill either so I would call it intuitive Vern. A lot of the moves mirror those I'm used to seeing my CAM software output so I would know what the spindle was supposed to do.

The part is less than 3/8" long (high) and I learned I could get 5 of them out of one length of stock with 4" of alum protruding from the collet. Using cut and paste I copied what I've posted here four times giving me four iterations. I know this is a great opportunity to use sub routines but I thought I had enough to sort out without further complications.

I handled the progressive step downs by using the tool length offsets in the Haas. T2 H02, T2 H116, T2 H117, T2 H118, T2 H119. H116 through H119 stepped down the length of the part plus the width of the cut off tool.

The XY offsets were done with multiple Gxxx's In the future G12 will probably work better for the vertical tools but the turning tools need to be fine tuned and I think different machine offsets will make small adjustment easier than changing the program.

I have not included a picture of the plate I mounted the tools too because it's a clone of Matt's which is pictured earlier in this thread. Matt was nice enough to post a program he wrote for his use in this thread and I copied it profusely. The only thing original in my effort is the resultant part.

The parts are about as simple a lathe job as you can get but were a real boring pain in the a** on my manual. It took me over 8 hours on the manual to make 200 of these and less than an hour (excluding programming and set up) to do them on the mill. I won't embarrass myself by telling you how many hours went into making the tool plate and sorting out the program. Suffice it to say I might break even if I make a couple thousand of these.

The parts are interlocking hats that capture a piece of carbon fiber from both sides. The program for the second hat is almost identical with the exception of length and minor diameter.

%
O01234 (LITTLE HAT)
N100 G20 G40 G49 G80 G90 G18 G00
N101 T2 M06
N102 G43 H02
N103 G124 Z8. (GET OVER TOOL HIGH )
N104G00 X0.475 Y0 (MOVE .475 OFF CENTER)
N105 / M08
N106 S4000 M03
N107 G00 Z1. (1" ABOVE TOOL)
N108 G00 Z0.05 (LEVEL WITH BOTTOM)
N109 G01 X0.425 F25. (MOVE IN TO .05 OFF PART, SET FEED)
N110 X-0.052 (TAKE FIRST FACE CUT)
N111 G00 Z0.1 (PART UP .1 FROM TOOL)
N112G00 X0.425 (RETRACT TOOL)
N113 G00 Z0.05 (LEVEL WITH BOTTOM)
N114 G00 Z0 (POS FOR FACE CUT)
N115 G01 X0.425 F25. (MOVE IN TO .05 OFF PART, SET FEED)
N116 X-0.052 (TAKE SECOND FACE CUT)
N117 G00 Z0.1 (PART UP .1 FROM TOOL)
N118 G00 X0.425 (RETRACT TOOL)
N119 G00 Z1.
N120 M09
N121 M01
N200 G20 G40 G49 G80 G90 G18 G00 (DRILL .3125 HOLE LITTLE HAT)
N201 T2 M06
N202 G43 H02
N203 G128 Z6. (GET OVER TOOL HIGH )
N204G00 X0 Y0 (CENTER OVER DRILL)
N205/ M08
N206 S3300 M03
N207 G00 Z1. (1" ABOVE DRILL)
N208 G00 Z0.05 (.05 ABOVE DRILL)
N209 G01 Z-0.44 F20. ( DRILL HOLE)
N210 G00 Z0.05
N211 M09
N212 G00 Z1.
N213 M01
N300 G20 G40 G49 G80 G90 G18 G00 (C-SINK .3125 HOLE )
N301 T2 M06
N302 G43 H02
N303 G129 Z6. (GET OVER TOOL HIGH )
N304 G00 X0 Y0 (CENTER OVER DRILL)
N305 / M08
N306 S200 M03
N307 G00 Z1. (1" ABOVE DRILL)
N308 G00 Z0.05 (.05 ABOVE DRILL)
N309 G00 Z-0.14
N310 G01 Z-0.155 F3. (CUT CHAMFER)
N311 G00 Z0.05
N312 M09
N303 G00 Z1.
N304 M01
N400 G20 G40 G49 G80 G90 G18 G00
N401 T2 M06 (CUTTING DIAMETER)
N420 G43 H02
N421 G00 G124 Z6. (MOVE TO TOOL 2)
N422 G00 X0.475 Y0 (MOVE OFF CENTER)
N433 / M08
N434 S4000 M03
N435 G00 Z1. (1" ABOVE PART)
N436 G00 Z0.05 (.05 ABOVE PART)
N437 G00 X0.29 (MOVE UNDER FOR 1ST VERTICAL CUT)
N438 G01 Z-0.265 F25. ( 1ST CUT)
N439 01 X0.425 (BACK AWAY)
N440 G00 Z0.1 (MOVE UP)
N442 G00 X0.21 (MOVE UNDER FOR 2ND CUT)
N442 G01 Z-0.265 ( 2ND CUT)
N443 G01 X0.425 (BACK AWAY)
N444 G00 Z0.1 (MOVE UP)
N445 M09
N446 M01
N500 G20 G40 G49 G80 G90 G18 G00 (PART OFF)
N501 T2 M06
N502 G43 H02
N503 G125 Z8. (MOVE TO TOOL 3)
N504 G00 X0.475 Y0 (MOVE .475 OFF CENTER)
N505 / M08
N506 S2000 M03
N507 G00 Z1. (1" ABOVE TOOL)
N508 G00 Z0.05 (.05 ABOVE TOOL)
N509 G00 Z-0.444 (POS FOR PART OFF)
N510 G01 X0.425 F3. (MOVE IN TO .05 OFF PART, SET FEED)
N511 X0. (PART OFF)
N512 G00 Z0.1 (PART UP .1 FROM TOOL)
N513 G00 X0.425 (RETRACT TOOL)
N514 G00 Z1.
N515 M05
N516 M09
N517 M01
(REPEAT 1)

Fire away, :)

Vern

More or less equivalent to how I would have done it back a few years when I was feeling my way through. I did the copy/paste until I became comfortable with subroutines. I put in laborious comments so I could figure out at a later date what I had done.

You will know you are making good progress when you start finding the comments annoying in a few months/years time and delete them all.

Hi Vern,

Nice to see that you got your lathe/mill working. Isn't automation GREAT!

Congratulations!

Vern,
Do you realize it is almost 10:30 :D

I just found this thread, very interesting, lots of great (new) input and I did read every last one of them, that wasn't fun but it was interesting.

Vern, Not wanting to be pushy but in post #9 you did mention something about investing in a video cam :D


Ken

Well done Vern! Don't be hard on yourself for taking hours to write that code. Everybody here started the same exact way. It's a new language to learn and, while simple once you understand everything, takes awhile to get comfy with. Soon enough you'll be able to glance at a few blocks and know exactly what's going on. I'll let you know when I myself get there. :) Relying on CAM like I do makes the learning curve longer, but it'll come either way.

Even though you may have taken a loss on these parts due to programming and staring-at-the-monitor time, you've gained that much experience. I do the same thing all the time since I don't have enough work to keep me busy enough for me to worry about. I'm constantly trying something new, and the next time I have a similar problem or job, I'll be that much better.

The parts look great, by the way.

Automation is a very mixed blessing because it comes with multiple languages of it's own. My recent purchase of the Haas Renishaw package brings the inscrutable hieroglyphics of macros with it. The probe and tool setter are great accuracy enhancers and speed up the set up many fold but that's only a small part of what the system will do, the rest is hidden behind macros, scaling, and orientation.

I purchased the Haas so I could make neat stuff, making money was a low priority. I've had the machine a little over a year and I can see the priority I gave making money with it has to be pushed even further down the list. :D

The real problem lies in my inability to leave well enough alone. The project in this thread as well as the Renishaw are examples of playing around with the fun stuff rather then concentrating on what makes money. My wife describes me as a geriatric teenager.

I appreciate the encouragement and consider the project a success, now all I have to do is forget the macros for a while and make some stuff with the Millathe. :)

Ken, sleep deprivation can lead to impotence and erectile dysfunction. :nono:


Vern

Heey everybody.

When I read this thread I got very exited so I tried to experiment a bit:

YouTube - Emco pc mill 50 turns into a lathe


I cant get mach to do a radius in the x-z perspective so I've done some straight lines. keeps giving a fault message referring to the K command.

(instead of using I...J... I used I...K for the radius definition)

But Ill keep on trying, Its nice to use my mill as a lathe, maybe in the future I buy a lathe for my workshop.

Greetz...

Nice Work Binski,

You guys are amazing. Just watch those fingers as they are in limited supply.

John

Haha thanks!

I whas only turning/milling pvc, no sharp moving points hahah.

I too have been struggeling to make a G code, I couldnt get bobcad to make a toolpath for roughing and getting the z axis to make a radius with the x axis.

So i made the toolpath by hand and no radius..

I'll keep practising though.

......I cant get mach to do a radius in the x-z perspective so I've done some straight lines. keeps giving a fault message referring to the K command........Greetz...

Did you use G18 to select the X Z plane?

Heey Geof,

You were right!

I forgot all about the G17/G18 .
I'm a bit of a newbie with programming in iso.

Here's the result:

YouTube - Emco pc mill 50 turns into a lathe vol2

Now to find A G-code for roughing and profiling....

......Now to find A G-code for roughing and profiling....

That is one thing missing on the milllathe; no G71, 72, 70. And no tool comp in G18 or G19.

Sorry I'm bringing back topic, but I have a question.
If I get X3 mill, what is bolt-on solution for chuck to use it as a lathe?
Is it possible to move table all way to the side so I can have longer workpiece?
How long of a workpiece I can handle with X3 mill using it as a lathe?

I don't have X3 mill, but thinking buying it as my first machine.

If you do my Z-mods you can move the head right down to the table.
The original configuration is limited by the ridiculously short gas strut.

http://www.cnczone.com/forums/showpost.php?p=438154&postcount=3
http://www.cnczone.com/forums/showpost.php?p=397011&postcount=4

Make or buy and R8 Arbor with a small faceplate on it and borrow the chuck from you 4th axis, or you can just use your collets.
It is possible to put a spindle interrupter so you can do threading.
To do it easy mount it behind the chuck, on the quill with a clamp.

Make a special Mach3 file and use a Machturn configuration.
Some channel's will need reconfiguring for the existing pinouts.
Like X becomes -Z, Y becomes -X and your original Z can be allocated to an extra channel - call it Y,A,B or C and that becomes tool height.
Or just leave it as a MILL and call it a horizontal borer.

It is OK for surface grinding too. Don't limit yourself.
http://www.cnczone.com/forums/showthread.php?p=486134#post486134

Don't worry that you can't make long things. Buy a cheap lathe, or mill it slowlyyy........... in your 4th axis between centers.
This makes a good machine for making tiny instrument size parts.
You can still probably make reasonable length parts. ER11 collets hold tiny parts really well.
The only limit on diameter is when the part hits the column, and by then you won't have enough torque to turn anything but wood anyway.