Applicable versions of OneCNC:


Description of situation or difficulty:


The solution was:

There are always ways of doing things that are pretty much undocumented. In my case, the solution is often embarassingly simple, but I still had to make that phone call in to support :D

So, just quote the above form and fill it in with what you learned. Try to keep it simple, one "revelation" per post, but post as many discoveries as you like.

Applicable versions of OneCNC:
One2000 Mill, likely OnecncXP

Description of situation or difficulty:
Trying to create minimum toolpaths for a near net shape workstock.
Even in a near net shape situation, I always like to rough cut, just in case there is a heavy stock zone, then finish cut.

I know I get stuck in certain modes of thinking and I always think, I've got to use the rough pathing before I use finishing pathing. Not so. :D

In this case, using Onecnc's roughing paths gave me more toolpath than I needed, or none at all, depending on whether I picked the roughstock boundary or the part boundary.

The solution was:
Use the finishing paths routines instead. You can still offset to leave another pass for a second cut later. In essence, you will get two finishing toolpaths, but you can always rename the first one in OnecncXP's NC manager.

Lesson: The finish routines give you a "net shape" toolpath with no extra stuff to clean out of an extents box, which is what roughing is designed to do.

Applicable versions of OneCNC:
Mill2000, likely OnecncXP

Description of situation or difficulty:
milling everything down to a certain level and no farther

The solution was:
This one isn't fresh in my mind, but here goes: at first, I was trying to use custom cuts. Custom cuts is necessary if you want to save time and machine exactly to a given plane, such as may exist in the part. Particularly in roughing, you need to make use of custom cuts to ensure that you don't leave a heavy stock above a certain plateau that may exist between your depth of cut options.

But custom cuts does not limit the downward toolpath creation. In this one situation, I needed to go back in and just alter the upward cusps of a mold project. What you need to do in this situation is sketch out a rectangular plane and surface it. Translate it right into your model to the level that you want to cut down to. I'm a bit hazy from here on, but I think you select your model to create toolpaths as per usual, and then select this planar surface as the boundary. Nothing will be re-cut below it.

HU,
In your post on milling down to certian level, you are working to HARD.
There is no need to add extra surfaces.

All you need to do is when you get to the section in the tool wizard that ask for automatic extents options is to uncheck the automatic z offset. This will ungrey the z offset option boxes. Then you can enter the depth that want to be z bottom of job and OneCNC will only mill down to that level.

WMS, I'll certainly keep that in mind, but without trying it out, I cannot be sure if I tried that and didn't like it for whatever reason.
Hmm..... the ideal method would result in rapid moves across the bottom where no machining is intended. Do you know off the top of your head if any method can do this?

HU,
I don't know if what you are asking for is possible.
Do to the fact that the program for safty reasons only makes rapid moves at clearance. And I can say I under stand why.
Thats not to say that I don't agree that it would be nice to do it exactly the way you are suggesting. I think that to error on the safe side is probably the way to go.
I have myself made the mistake of tweaking code only to find that now the tool goes thru the part instead of around the part. Not good.

No no, I should have qualified my statement, since a rise to clearance is okay. I'm just wondering whether some methods will cause the tool to feed all the way across the "false bottom"?

HU,
I'm pretty dense, do you mean a false cavity bottom or around the outside of an island (for lack of better word)?
If you mean a cavity bottom, it will be machined (ie: feed) just as if your false bottom was in fact the real bottom.
Around the outside would depend on what was in the way(ie: it would see the model parts and not go thru them) so it might go to clearance before it moves.
Maybe I don't understand the question. If not try to set me staight.

Yes, I mean a false cavity bottom. On behalf of One2000 owners, this would be valuable to know how to make it "skip" the false bottom, by rapids to clearance. The Rest Robot can likely be used in the OnecncXP to accomplish much the same thing.

Maybe Onecnc can also jump in here and clarify this officially, once and for all. But if you know, post away. :)

HU,
I guess I still don't quite understand the question. I told you I was dence.

I'll try to clear up my thoughts.

Let's say you have a cavity that is 2 inchs deep, with tapered or radius walls at the lower half. And you want to use a 1 inch mill to do the top half but it won't fit into the bottom half.

You can set the extent box to a end depth of z-1.0 (or let the program figure out how low it can go)and then when you go back at it with say a 1/2 mill on step #2 you can set the extent box to start at say z-.975 and end at the defalt value(ie: z-2.) or any other value you chose.

That way the 1/2 mill will not recut the area the 1 inch mill already removed.

This work for both Mill2000 and XP.

This applies to solid model not 2d pockets.
As 2d pocket are bound by the outer boundarys that you pick and the software has no way to know that the area under the top boundary differs from that top boundary.

Visualise something like an egg carton, all peaks and valleys.

If you had already cut the entire 2" deep mold with a 1/2" diameter ballnose and then you wanted to recut just the top 1" of it over again because, say they had cropped the top 3/4" of the model, and reskinned it (its not just a flat plane top, but is 3d), then you would want to save time by not going all the way down to the bottom any more, but would just want to rapid across the open areas until you get to the islands (this is finish cut only), start at 1" depth and come back up and mill the detail on the island plateau. Am I getting close to making myself clear yet? :D

Murry,

I don't think this is possible as the program thinks there is material to come out any where withing the measurements of the extents box. As you say maybe the rest robot in xp will do this for you, I don't know nor can I check. You can however set a z bottom as wms said on the last page of the tool wizard, just change the z depth to what you want. I do this all the time as I machine half the part from one side, turn it over and machine the other.
Ken

Hu,
I think we are both thinking about the same thing. Just saying it differently.
If you set the extent box to start at Z0 (or some clearance) and
then set the end Z-1.00 it will force the tool path to stay above Z-1.00 and will not machine below that level.

If you use z level finish it should retract to clearance and move to the next peak or valley.
If you use z level rough it will asume that there is material everywhere (ie: solid stock) and will machine it that way.

HU, kind of like this?

wms,
bingo, couldn't have said it better myself.

Ken

I get it now I think, when you said use Z level finish. I got caught on that again. :D

Applicable versions of OneCNC:
OneCNCXp all types

Description of situation or difficulty:
Special user setting for different work

The solution was:

I got to thinking about the user setting and how to apply them to different kinds of jobs rather than different users per say.

For instance:
Mold work setting could go like this:
user name:molds (you could set up different types of mold too)
Then you could customize the setting to fit the work.
Layers = top plate
bottom plate
pull pins
counter bores
top cavity
bottom cavity
reverse ingraving
ect.........

you could even edit the tools and material library to match the work.


aerospace work setting.
user name: aerospace

Layers = stock
webs
material counterbores
ods
bores
tabs (to be removed)
ect......


High speed milling setting.
user name: high speed milling

layers =


This setting would be a good place to edit he material setting to reflect high speed milling parameters as they are so different from regular miling.

These are just examples of what you could do. It's the idea I'm trying to present here. That you could save yourself some time and trouble if you do different types of work, by setting up different setting to match the work.

That sounds like a good plan, WMS, but where do you see the option to set up several different individual user settings within the program? I must have missed that part.

Hu,
It's when you first open up OneCNC from your desktop. (XP only)

Bear with me, but you mean the little drop-down dialog that says default? How do you change it to something different? Is this referring to default user?

HU,
Thats right . You can set up different "users" at this drop down, each will have it's own unique setting. That is, different layer structure, material list, tool setting, color choises, tolerance, toolbar docking, ect....
Basically any thing you can modify in OneCNC.
Pretty cool. :cool:

And so you don't have to start from scatch, you can copy your personal setting and rename them to the new acount. Then modifiy the things you want to change.
I'm sure you already know that these setting are located in the OneCNC file: OneCNC-xp/mill expert/setting/users/default (or any named acount you have set up)

Originally posted by wms
HU,
snip
I'm sure you already know that these setting are located in the OneCNC file: OneCNC-xp/mill expert/setting/users/default (or any named acount you have set up)

Dammit, WMS, you are wrong again. I didn't know that :D :D

Its a good thing to have these discussion boards!!

Hu,
I havn't finished that big bucket of crow yet, want I send some up your way? I did get all the egg of my face though.:p

Applicable versions of OneCNC:
OneCNCXp all types

Description of situation or difficulty:
Needed a way to wrap lettering around arc then extrude.
In XP there is "Chain text" funtion to wrap text around an arc. But this funtion vectoizes the text when it applies it to the chain.
So this text is not a surface. So it is not possible to use the extrude font funtion under solids maker button.

The solution was:
1: Use the "chain text" funtion.
2: Then in the surface menu, use the " surface from curves" funtion to surface the individual letters.
3: Then in the solids menu use "Extrude surface" funtion.


(Thanks to Mike Reyes at OneCNC for his help on this problem):D

Keep the articles coming, WMS, we're reading :)

Thanks Hu,
Good to know someone reads these ramblings. Hope you can glean a small amount of info from them.;)

Applicable versions of OneCNC:
Xp vesions

Description of situation or difficulty:
Needed away to machine an island with one or more "keys" around it. This is kind of hard to explain so follow along.(If you want)

The solution was:
A real mind bender
Radial roughing and Radial finishing.
As follows:
I used file mill steep wall machining inch.xfa as a mule file. It's in the sample files at xfa/samples. If you want to try this yourself.

Open up the file and
1) Extract a curve, the top circle. (see photo 1 wire frame)
2) Create a point at arc center. (the aqua one in photo) you need this later for start point.
3) Open up nc manager and start a new tool group. Number #2.
Highlight the new tool group by clicking on it.
4) click on the model toolpath button and select "smt rought"and "z level" .
5) select ramp, 2 degrees, climb mill.
Then select 1 inch mill.
At the cut option box, set minimum for finish to .060 and step over .500 and depth of cut to .075.
At boundary setup box check the extents box and the normal box.
Boundary of toolpath, leave the automatic boxes checked. (it will figure out were it needs to go)
Now wait...... whistle if you want..........while it crunchs numbers.


6) click on the model toolpaths again and select "smt finish" and "radial"
7) select the point you created at the start.(see I told you you would need it.:p )
8) Now select a 1/2 ball mill.
9) when you get to the "radial option" enter start angle 0 degrees and step 1 and included angle 360. then leave for finish .050 and suface tolerance .0002.
10) At the boundary box: check extents box and normal.
11) boundary of toolpath same as before leave the auto boxes checked. click finished and wait.......whistle some more......crunch, crunch, crunch.

12) click on the model toolpaths again and select "smt finish" and "radial"
13) select the point you created at the start.
14) leave the tool the same as before. (1/2 ball mill.)
15) when you get to the "radial option" enter start angle 0 degrees and step 1 and but now included angle 270. then leave for finish .000 and surface tolerance .0002.
16) At the boundary box: check extents box and normal.
17) boundary of toolpath same as before leave the auto boxes checked. click finished and wait.......whistle some more......crunch, crunch, crunch. better go get somthing to eat....

Now for the fun, select tool group #2 then post, then simulate, leave the stock size auto box checked, (again it will figure it out) set the slider button to about half way between turbo and slow. Click on ok, and eat what ever you went to get.......crunch....heavy math here......

And you should have photo #2.(rendering)

This is only an example of what you can do. Let's say you needed to put 10 keys around you island, You could do that. By radial cut that start and stop at different degrees on your model.

The hard way to do this same thing would be to construct all kinds of different sufaces or solids and merge and cut and merge and cut. Better to do it the Easy way.:D

Sorry photo #1 didn't get attached to the post above. .

So here it is.

Here's a tip if you are profilling a chain.

This is a pocket in a part that I needed to run a .050 corner rad mill around. I didn't want to spend the time to finish mill the radius with a ball mill. Onecnc will do that very thing. But sometimes it makes more sense to just use a rad tool.
You can't see all the pocket but it has radius at all corners as most pockets do.

If you look real close( sorry the pics are not better, hard to get lots of info on to screen), at the top picture you will see that the ramp on to the chain (green tool path) is outside the actual toolpath. Here I picked the Red line as the start of the chain.

If you look at the bottom pocket you will see that I broke the line in two, with divide, and picked the Red line there as the start of the chain. The second one is lots better as it ramps out in the pocket as opossed to in the corner. Here there is plenty of room for it make its move with out any interference.

You also can adjust the radius in / out to different setting to help in these situations.

Good tip, WMS. Sometimes I find it's so easy to miss the simple solution :)

Thanks for resurrecting this thread, too. It was kind of good to review the contents of the rest of it.

Hu and WMS,

I think a nice addition to Mill Expert would be the ability for the software to automatically start the chosen pocket/profile at the midpoint of the entity selected for the start of the chain.

I use Mastercam for 2D profiling and this is a check box option which saves huge amounts of time having to do as WMS does-breaking the entity into two pieces (I used to have to do this with Smartcam years ago).

Maybe OneCNC can add this to the "want list"?

Mark Linder
(Alas, I have no cool Avatar yet)

What do you have in mind M, I'll find you an avatar

PEACE :D

Right on Mark. Good to hear from you!

Onecnc tech spport does read here, so I'm sure if there is nothing forbidding this from happening, that it could well show up as another feature.

Only this evening was I playing around with the merge function in Onecnc, when it dawned on me that not only can I merge a CAD drawing, but also, its CAM information comes in with it. Granted, at this stage, the incoming file must have its components located in the proper place, so maybe this does limit what I am imagining doing. But the possibility exists for sort of a library of premachined features.

Maybe other guys knew about this and were hiding it from me. ;)

Hardmill,

I will definitely give it some thought. Thanks for the offer!

Once I define the persona I would like to convey here, you'll be the first to know.

You would need some kind of jpg, gif, or such for creating it, right?

By the way, being more or less a 2D (Mastercam router) guy who recently bought OneCNC Mill Expert, I have already learned so much useful info on how to use Mill Expert from the contributors to this board.

Hopefully, I can add some useful tips/tricks and offer insight on various relevant subjects.

Mark Linder
(soon to have an avatar!)

Hardmill,

OK. I have a pic I would like to use for my avatar. It is 150 x 150 pixels, though (needs to be 85 x 85?). I have attached it for you to check out.

Yep, I like to ride quads in the desert. I live in the San Deigo, CA area and miles and miles of dunes are only an hour and a half from my home.

Let me know if you need anything else.

Thanks!

Mark Linder
(Oh, so close to having an avatar, now!)

I did it for you.

Glad to see you found one.
PEACE:D

MY LIFE IS NOW COMPLETE!

Thanks a lot you guys.

Mark Linder

Ummm, I meant San Diego - not San Deigo.

You would think I would get that RIGHT after 44 years. Geez.

Mark

OneCnC XP series (may apply to 2000 series)


Here's a little tip if you like me use dwell in your drill cycles. Or any other cycles.

If you enter 300 (no decimal point) in the dwell box. You will get 300. (with a decimal point) in your posted code.

This changes the dwell time from 300 milliseconds to 300 seconds.
That's 5 minutes guys.

But if you put a "space" after the 300 ( no decimal point) then it outputs 300 no decimal point.

Much better:D

If your control needs the decimal point then you only need to enter the number.




Thanks to James at onecnc au for the tip.;)

Xp and 2000 series.

In an earlier post Hu was asking about verify one or two funtion and how it can sometimes make your scratch your head. I suggested that he use "tape measure".

I have also found that is you go to a normal view, (top, side,front,ect.) you can use the dimension funtions to verify entities that are not on the same plane.

Say you have a line that is at Z zero and a hole location that is at Z -.500. If you select top view and use dimension, horzontal or vertical, (depending on the entites) it will give you the distance in that plane. So you can check things to see if they are where you want them. Then just use the undo to remove the dimesion.

The "tape measure" measures end points so sometimes it's not what you want to check. Between the two you can find about anything you need to know.

I would like to see right click context sensitive menu on the drawing section of the screen. For example, after importing drawing data (that seems to ALWAYS be on the same layer as the part geometry), the ability to select the entities to delete, then right click - select "delete" from the right click menu, and say bye to the selected entities. It is a little thing, but it sure saves time in a lot of case. Maybe the ability to change the attributes of the selected entities - such as color, layer, etc.

I am sure I (we) could come up with several other things that might make a context menu meaningful.

Any other ideas?

Mark Linder
(Sweating his balls of his feet off in sunny San Diego, CA)

Yes, I'd have to agree with you, Mark. My RMB could be busier :)

HU,

Here's another.

When you draw something, or want to move an entity, or group of entities, the coordinates dialog box offers many types of ways to move. I would like to see simply "origin" added to the list, so one doesn't have to enter "0,0" all the time. (I hope that made sense).

Another one of those small but time saving things.

I always like to put a point a 0,0,0 Then when I want to move to origin I just use the from point to point selection.

Mortek,

Thanks for the tip!

I will try that out.

Mark Linder

Since I'm getting more into solid modelling, I look for a way to save a little time when I can.

I think the function "surface from curves" can be used for completely seperate loops, such as turning a 2d hole pattern into circular planes in a batch, without picking a border that contains the whole works.

For example, the function "Draw hole pattern" gives you 2d arcs of course, but you can quickly turn all these into circular planes by using "Surface from curves" and pick them all, assuming that they are all in the same plane.

This makes all the individual circular planes behave as one surface, so be sure to use "Disconnect surfaces" before you extrude them into cylinders, otherwise, the program will likely crash.

Hu,
Great tip! Now I can draw that Pipe organ I've always wanted to.:D

Lots of neat tricks in the software. Easy on the user.:p

Hey guys,

When you use rest machining in one xp, does the rest tool go over the entire part again or only create toolpaths where needed to clean up?

Hey Ken,
It only creates tool paths for the stuff that is more than your tolerance. Say you set it for .002 as your tolerance, it will find the spots that are more than .002 and create the paths to clean these areas up. So it only hits what is necessary to get to your tolerance.

Ward,
When you do z-level finishing what do you set your tolerance to. I have had mine to .0001 to try to tighten up circular finishes, but I find that the program thinks there are discontinuities in the surface so its not creating uniform constant step down paths. In other words the cutter will jump out of the part when it should keep going x or y. Then the next time around it will rapid down to the next level where it pulled out. Any thoughts?

Ken,
Under properties, set your genearal and chain gap to.00039.
Under your tool "cut options" set to .0016.
That sould be about right.
I use this setting for Mill 2000 and the parts are a smooth as a Baby's Butt. No hand finishing at all.

This is different than the rest machine tolerance. But I guess you know that. ;)

Originally posted by Mortek
Ward,
When you do z-level finishing what do you set your tolerance to. I have had mine to .0001 to try to tighten up circular finishes, but I find that the program thinks there are discontinuities in the surface so its not creating uniform constant step down paths. In other words the cutter will jump out of the part when it should keep going x or y. Then the next time around it will rapid down to the next level where it pulled out. Any thoughts?

Hi Mortek,

I've kind of run into the same situation and I think it has to do with how much the toolpath is an approximation of the surface. I think the surface accuracy itself is carried to something like 16 decimal places. So, when a chord is drawn across two points on the surface, it is conceivable that you could have that much of a "hump" in the surface between those two endpoints, of .0001 or more, because you are trying for a longer segment length to keep the program flowing at a decent rate through the control.

As an experiment, try setting your "amount to leave for finish" to a small amount like .001 or .002 and don't change anything else. See if the rapid up and down is eliminated that way.

I suppose a person should work at 10 times the accuracy in the model that you are going to machine at, just to eliminate these glitches that arise by trying to force extreme toolpath precision which is equal to the model's precision. Something's got to have room to get rounded off.

That is my current 2 cents worth, and I may be totally out to lunch. That's how we get experienced, though, isn't it :)

I tried what you said leaving .001 or .002. It didn't help. In fact it may have gotten worse. Do you think it could have anything to do with how you create the surface? You know by picking borders or cross sectional or 3 sided surface etc. ? I am cutting with a 1/4 ball mill hanging out 3" and every time it rapids out and in I get a little chatter on the wall. I would love to get it to quit. Do you find this happening in XP. Has the new SMT tool pathing helped this?

Originally posted by Mortek
Ward,
When you do z-level finishing what do you set your tolerance to. I have had mine to .0001 to try to tighten up circular finishes, but I find that the program thinks there are discontinuities in the surface so its not creating uniform constant step down paths. In other words the cutter will jump out of the part when it should keep going x or y. Then the next time around it will rapid down to the next level where it pulled out. Any thoughts?

Ken,
You say it moves down were it pulls out. Are you using vertical or radial aproach on your z-level finish?

If you are using vertical, this may be the problem if the part wall has any taper to it.

If you are using radial, did you sketch a start point or let it figure ou the start point?

I've been using vertical, the wall are straight up and down at this point. Radial won't help on it's way out of the part will it?

I was experiencing exactly what you described when machining near the vertical wall of the impeller hub I posted about. At first, I had an inner boundary set to exactly the same diameter as the hub OD. When I went to finish cut, the first pass was a series of plunges and rapid returns all around the circumference of the hub. I had to adjust the inner boundary to be .0015" outside the vertical wall to make this cutting action change into a smooth circumferential orbit.

I am reasonably sure that this happened because I created the model with not too great precision. This resulted in my curves not being as smooth as they could have been. So I speculate that the angularity of my model creates interference with the toolpaths, which forces gouge checking to cut in, and then forces the tool into plunge mode. It cannot make the move in XY from point to point because it is calculating that the "inviolatable surface" protrudes (just a hair) between the two points.

So somehow, I think you'll have to discover where this boundary distance is in your situation. With an extreme tool overhang as you describe, I can imagine the thing is continually being twisted off center whenever it cuts and it may not return to perfect centeredness between cuts.

What else could you try? Try using Z level roughing (zero to finish) and force a cut at the level you want to work at to create this fillet. Maybe this will keep the tool down for the duration?

Ken,
It hard to envision what you are saying, with out being there. But I would try thre radial aproach and see if it will help.

The vertical aproach will step straight down and this may be causing the chatter. As the tool comes to a stop, then steps down, probably at 1/2 the feed speed, it could be unloading the tool. This would cause it to chatter.

The radial aproach would move off the part, at normal feed, and then step down, in free space, then move back onto the part. Again at normal feed.

Sure worth a try, especially with so much tool hanging out.

Okay, just tried radial approach, zoomed in on one of the places that it is coming out and it doesn't radial depart.

Ken,

On the computer or on the machine?

What do you mean coming out?

I zoomed in on the toolpath on the PC. By coming out I mean rapiding to Z clearance before finishing the xy toolpath. Do you know how to make a JPG. file small enough to post a picture of the toolpath? Every time I try to print screen, paste it in paint. crop out what I want and paste it in a new paint screen the image ends up to large to post.

Ken,

Here http://www.cnczone.com/showthread.php?s=&threadid=600

I'm wondering in which cases radial approach works in z-level finishing. It appears that if you are restraining the toolpath by a boundary that it seldom works. The Help files say that if there is room then the radial approach IE depart will work, but if not room it defaults to vertical approach.

I was able by changing the way I finish the rest of the part, to shorten my tool stickout to 2.5 inches. I seem to be getting a good finish and by allowing .002 stock I am avoiding gouging the already finished surfaces even though it's defaulting to vertical approach>

Ken

Hi Mortek,

I use a screen capture program called 5clicks to take screen shots. As you have found out, windows bitmap format is huge when using print screen to Paint.

I think you can use "5 clicks" for 30 days free, then you need to register, but it is well worth it. Most screen shots saved in png format are less than 70k, and look better than jpg.

I have a few imcremental macros that I have figured out for thread milling. I have these set up in custom code, but I was puzzling about how to make a neat insertion into the NC manager, in the event that I had a several holes to do.

The method I used was to set up a special machine cycle which I call thread mill.
Start lines:
{/X}{/Y} 'movement to first hole

Mid lines: call the macro
/N (Bandit subroutine macro call)
{/X}{/Y} 'move to next position

End lines
/N (final sub call)
N (unconditional jump in main program, Bandit style)

I call this special cycle then, just like any other drill cycle, and then insert the custom macro code after it, a simple 2 step process in the NC manager.

When I post the code, my subroutine macro is posted right inside the main program body. After posting, I then have to find the appropriate line number for the start of the macro, and paste this after each instance of "/N".

Then, I find the line number of the line following the end of the macro, and paste that in after the "N", which in Bandit code, forces the main program to skip ahead past the macro in the main program, when it gets to it. Thus, the main program can execute smoothly afterwards for subsequent processes.

I don't know if this will help or hinder anybody, since most of you use ISO code. But, it works better than just plopping gobs of macro code into your program, because then the NC manager's normal method of laying out the code for this tool, etc, will come out neat and correct, with a minimum of fuss.

I posted this on the other board. But I wanted to post it here as well. Enjoy.

Guys,

Here's a tip that Bob F. turned me on to when selecting edges to fillet.

After you select the fillet function and you start to go around the part to select edges, you can zoom in or out, with out "losing" the funtion, by placing your curser over the area you want to look at and press the "+"(plus key) to zoom in and the"-"( minus key) to zoom out.
This way you can zoom right in on your edges and make sure that you select all the ones you need to make fillet work.

Where you place the cursor becomes the center of your screen.

This works on both Xp series and Mill 2000/2004.
And in Xp series you can use the wheel on the mouse to rotate the part with out losing the funtion.

This may work for other things as well.

Pretty cool stuff.

Thanks Bob for the tip.

WMS,

Is this something you have to turn on somewhere? I just tried it in ver. 4.36 of Mill Prof 2000 and could not get it to work no matter what I do.


Okay I take that back. The"+ or -" Key on the number pad of the keyboard works.

Ken

Originally posted by HuFlungDung

I don't know if this will help or hinder anybody, since most of you use ISO code. But, it works better than just plopping gobs of macro code into your program, because then the NC manager's normal method of laying out the code for this tool, etc, will come out neat and correct, with a minimum of fuss.

If there is one thing I've learned from Hu, it is "don't buy anything with a bandit controller".

It seems you spend more time messing around with the programming than cutting material.

I'm so glad I have a machine that reads straight forward G code and macros without any propriatary weirdness.

You are quite right Keith, they do take some fooling with, because they were originally built on a competitive system to ISO, but then they aren't nearly as tough as some of the "conversationals" that I've seen guys working with (trying to create Gcode posts)

Bandit is pretty much extinct, anyway, and service and boards are hard to come by, but the Shadow came along so that "something" would be able to run existing programs. It is kind of the "inbetween stage" between the homebuilts the guys on these forums are building, and big name cnc's.

But, it moves the cutter in all three axis, that's all I care about. Its actually very handy to run, if you like living on the edge: it will execute any line of code you give it without a big song and dance first. :)

:) hi keith
thats the thing i love about ONECNC
no matter if you have a old controller
or a new controller
onecnc is flexable in posting toolpaths to suit your controller
old or new
regards
peter:)

Guys,

Here is Link to a new "Third Party" book that is due to be released December 2003.



http://www.f1help.biz/ccp51/cgi-bin/cp-app.cgi?usr=51F2587890&rnd=2996215&rrc=N&affl=&cip=216.250.43.133&act=&aff=&pg=cat&ref=OneCNC

One of the advantages of being a hybrid CAD/CAM system is when dealing with imported models it is not necessary to Stitch or sew surfaces together for machining.

OneCNC CAD/CAM software recognizes tangent surfaces, even when not closed to form a water tight model, and allows machining of imperfect models by mathematically "healing" the model during import and then re-examining the model again during the generation of tool paths.

This ability is possible because OneCNC is built on solids originally, not as an after thought or third party add-on. So therefore OneCNC treats a single surface, or multiple surfaces as solids, even when their not.

This makes OneCNC uniquely capable of reducing programming time and so is easier to use so you can focus on programming, rather than wasting time repairing models.

With OneCNC its as simple as import and machine.

OneCNC LLC
(877) 626-1262
(813) 874-2335
www.onecnc.net