Emco Compact 5 PC and F1 with Welturn/Welmill

[dertsap]

I haven't tried fusion lathe posts so I can't be of any help there . But , I think that most fanuc type processors should work .
I've used the dolphincam lathe and it has a decent processor for the linuxcnc , which is why I had suggested it previously . I've run my lathe a few times since getting it up and going, but my mills keep me far too busy to do any of my desired lathe work , so I haven't had time to compare how well fusion 360 will work . Fusions cam for the mill seems pretty good and I'd imagine that the lathe cam is going to be as powerful .
If I can free up some time then I'll take a look at fision and see what they offer in regards to a post that would suite linuxcnc

Hand programming for lathes is fairly easy once a guy has a grasp of the coding . I suggest doing your best to understand g codes and how each one works .
G0 g1 g2 g3 are the most common codes used in programming and are good codes to learn and master
I work on hass lathes quite a lot and most of my coding is done at the machine and usually all hand programmed

[SharpShooterSer]

I haven't tried fusion lathe posts so I can't be of any help there . But , I think that most fanuc type processors should work .
I've used the dolphincam lathe and it has a decent processor for the linuxcnc , which is why I had suggested it previously . I've run my lathe a few times since getting it up and going, but my mills keep me far too busy to do any of my desired lathe work , so I haven't had time to compare how well fusion 360 will work . Fusions cam for the mill seems pretty good and I'd imagine that the lathe cam is going to be as powerful .
If I can free up some time then I'll take a look at fision and see what they offer in regards to a post that would suite linuxcnc

Hand programming for lathes is fairly easy once a guy has a grasp of the coding . I suggest doing your best to understand g codes and how each one works .
G0 g1 g2 g3 are the most common codes used in programming and are good codes to learn and master
I work on hass lathes quite a lot and most of my coding is done at the machine and usually all hand programmed

The inevetibility of hand programing is always there, just the canned cycles for a lot of stuff would ease it up a bit. Maybe getting some of the addons could make my life easier when trying to make a code for a complete part (I really dont produce too many parts, but its pita to do it on manual lathe, especially the ball/handle shapes, and threading).
I ve also read that Fusions emc2 p/p are great, and thats a relief - for the time when I get the lathe to listen to me and start throwing chips - and I move on to the mill as well. For turning, it seems no one has made a definitive full working p/p for emc2, all of them need some adjustments. But lets get one step at the time.
So for now, I have to get to the bottom of this.
For instance, one of the things I want to try is to cut a 1/2-20 unf thread, on 1 inch length.
I was thinking of following - to precut the part to desired OD. Use g7 g18 g20 in mdi just to ne sure.
Touch off the part ox x and z.
Then use this
G0 x1 z1
G76 p0.05 z-1 i -0.5 j 0.005 r2 k 0.02975 q 29.5 h 2 e 0.02975 l3

Maybe it will work?

[SharpShooterSer]

The inevetibility of hand programing is always there, just the canned cycles for a lot of stuff would ease it up a bit. Maybe getting some of the addons could make my life easier when trying to make a code for a complete part (I really dont produce too many parts, but its pita to do it on manual lathe, especially the ball/handle shapes, and threading).
I ve also read that Fusions emc2 p/p are great, and thats a relief - for the time when I get the lathe to listen to me and start throwing chips - and I move on to the mill as well. For turning, it seems no one has made a definitive full working p/p for emc2, all of them need some adjustments. But lets get one step at the time.
So for now, I have to get to the bottom of this.
For instance, one of the things I want to try is to cut a 1/2-20 unf thread, on 1 inch length.
I was thinking of following - to precut the part to desired OD. Use g7 g18 g20 in mdi just to ne sure.
Touch off the part ox x and z.
Then use this
G0 x1 z1
G76 p0.05 z-1 i -0.5 j 0.005 r2 k 0.02975 q 29.5 h 2 e 0.02975 l3

Maybe it will work?

Hm this seemsxto work, but I m off with a few digits, have to re run

[SharpShooterSer]

It does work! Just to figure the fine setup for not having this go this rough (or maybe it isnt that rough for the machine) the threads came out nice. The depth wasnt correct (at the end I used k0.075 and I was able to screw on the test gauge), but from the online thread size tables I wasnt sure which value to use to subtract from 0.5 inch. I m a metric user, but this is one of the thread sizes that I need to cut on my parts, thats why I tried it
This type of code can be inserted into another, with tool change, to get a whole operation going. Now to find the cycles that can help me get the desired shape, if there are any. It would be painful to write everything up,

[Fastest1]

It looks like you are coming along very nicely. I am guessing that video was with LinuxCNC? What did you have to do or how did you get it running correctly?

2 things about CncZone and its members in general.

1. is that they dont come to flame or insult. From what I have seen only to help. At times of course there are incidences where you must learn for yourself and there is a curve. It can seem impossible at times. Everyone struggles at some point.

2. Most likely not many of us were paying attention in writing classes. So proper use of punctuation, spelling and terminology is unlikely.

Somehow though even when we live in other parts of the world, speak different languages, have different religious beliefs etc. We still just want to help each other. In fact it seems to be just the opposite of most internet methods of communication where everyone trashes each other. Quite refreshing.

[SharpShooterSer]

Its with linuxcnc

I preprared the piece of material to be 0.5 OD (and jaws are as good as new so no runout), touch of x and z and in mdi gave the g0 x1 z0.2 command, then the following g76. it warned me that I should turn on the spindle (M3) and I did prior to this type in a g7, g18 and g20 just to be sure what I am doing.

the g76 i wrote by hand at first G76 p0.05 z-1 i -0.5 j 0.005 r2 k 0.02975 q 29.5 h 2 e 0.02975 l3, but later I changed the K to 0.075 , put the R to 1 H to 0, E is same as K and L0, to get it to do this faster. it took ages with the first line of code. And I set spindle speed at 550, its quite steady. I hope this wasnt too fast? I have to get to the bottom of these R, H and L , and also to find a proper table for depths of cut for the threads - used 0.075 was a pure estimate ( in some tables I found that minor diameter should be 0.46** something, I subtracted that from 0.5 and divided by 2 at first, way too shallow lol, then I just used the 0.5 minus minor diameter, that was too shallow too - perhaps I am using the wrong lines in those tables?)

[dertsap]

looks like a good start
I did a google search and it appears that there are a few guys that have modded fusion posts to work with linuxcnc , so there are some posts out there .
here is something fairly new and cheap eCam - Easy Cad/Cam System . I ran across this a while back and it seems to be fairly easy to use and functional . I'm not sure how well it posts but the demo might be worth giving a try

[SharpShooterSer]

yeah, there are a few p/p out there for fusion/emc2 but no one says its definite. when I get to it, I m sure I ll find the one that works perfectly with my machine.

I ve tried out eCam, its seems simple to use, and I ve generated the code, but there are some hiccups - for instance, I get a message that it doesnt recognize g96 (?), but there is vast number of lines with U (I have attached a file to check it out) - I dont know how did that get there maybe some of you can shine some light?

[dertsap]

I don't think that u or w are accepted in linuxcnc nor g96 , I may be wrong about this . It might be a good idea to contact them and ask if they have leaner simpler post processor that would work .
It should be fairly straight forward for them to do so . Heres a list of the codes LinuxCNC "G-Code" Quick Reference
Ive tried loading your code into linuxcnc , and no matter how much code I chop out I keep getting a /375 error on line 2 . Not sure what the deal is with that

[SharpShooterSer]

yeah, same thing happened to me I ll send them an email. Software seems pretty easy to use!

[dertsap]

I'm not overly experienced with cam programs for lathes . It's as I said before - most of my coding is down and dirty at the machine control and I can punch out a program fairly quickly .
If you can draw 2d in cad then your part way to hand coding even complex parts . All that is needed to create the profile codes are all the points for either line moves or arc moves . From there you can create and tweak needed roughing passes or what not . At least this would be a start until you get sorted with a cam package

[109jb]

U and W are axis words, as in X, Y, Z, A, B, C, U, V, W.

G96 is accepted and supported by LinuxCNC if the machine is properly equipped.

[SharpShooterSer]

You are right, its all in the setup for P/P. I am not comfortable with tampering with it too much, but I sorta got the code that can be read.

He pointed me out to https://tenacious.gitbooks.io/ecam/c...uidelines.html and https://tenacious.gitbooks.io/ecam/c...templates.html

This guy got it working


Now, the code I got to run in simulation on my home PC (not connected to a machine), called the adapter (attached) has feeds of 0.5 and 0.2. Looking at the simulation, it might be done in 2116 If I use F10 for instance (in second one) its not moving too fast also. Maybe because its not sensing spindle turning? I will try to be cautious with it, and try the slow one
I had to delete some of the codes (like g99, m3??? and writing in there, because I got the error messages). But we might be onto something here

[SharpShooterSer]

Tried it on a machine (note to self - do not attempt 0.5 mm or 1 mm plunge cuts on this small machine) and if I use F100. and F50. it moves woth normal feed speeds. Maybe I missed something about F beeing a % feature?

[RCaffin]

I have to get to the bottom of these R, H and L , and also to find a proper table for depths of cut for the threads

I don't think there are tables for this. It depends on material, diameter, cutter, pitch, phase of the moon, ...
I start off with a very shallow DoC and go up from there in test runs.
As a rule, and using an M8x1.25 thread just as an example:
OD: 8.00 mm
ID: OD-Pitch = 8.00 - 1.25 = 6.75 mm
If you are in imperial essentially the same thing applies.

BUT, depending on your threading tool, you may need to add or subtract a little bit. If you are using a pure 60 degree threading tip, you will have to go in about pitch/8 (I think), to allow for the rounded bottom to the thread profile. Yeah, it gets complicated. On the other hand, if you are using a genuine commercial threading tip DESIGNED for M8, you would probably use zero correction.

A spindle speed of 550 is maybe a shade high, but OK if your lathe has a fast saddle.

Cheers
Roger

[dertsap]

Tried it on a machine (note to self - do not attempt 0.5 mm or 1 mm plunge cuts on this small machine) and if I use F100. and F50. it moves woth normal feed speeds. Maybe I missed something about F beeing a % feature?

If you add a g95 to the code then you can use a feed / revolution which is in my opinion a better and safer method than ipm or mm/minute . Then your feed would look more like F.05 .
If you look in your ini file (configuration file)then you will see start up codes , you can add the g95 in there and it'll always be a default

[RCaffin]

If you are threading, then only spin signifies. The feed value is ignored. It HAS to be ignored after all.

Cheers
Roger

[dertsap]

I was talking about feeds in general not threading

[SharpShooterSer]

If you are threading, then only spin signifies. The feed value is ignored. It HAS to be ignored after all.

Cheers
Roger

I know feed is irelevant when threading, I was talking for general turning F. I use metric system (still everytime I start up the config I have to manually change it to mm and use g21) and fron the testing I saw that using 60 mm/min for steel on 1000 rpm sounds good while working.
The g95 sounds as a good idea for the future settings and work.

[SharpShooterSer]

I don't think there are tables for this. It depends on material, diameter, cutter, pitch, phase of the moon, ...
I start off with a very shallow DoC and go up from there in test runs.
As a rule, and using an M8x1.25 thread just as an example:
OD: 8.00 mm
ID: OD-Pitch = 8.00 - 1.25 = 6.75 mm
If you are in imperial essentially the same thing applies.

BUT, depending on your threading tool, you may need to add or subtract a little bit. If you are using a pure 60 degree threading tip, you will have to go in about pitch/8 (I think), to allow for the rounded bottom to the thread profile. Yeah, it gets complicated. On the other hand, if you are using a genuine commercial threading tip DESIGNED for M8, you would probably use zero correction.

A spindle speed of 550 is maybe a shade high, but OK if your lathe has a fast saddle.

Cheers
Roger

It looks like the moon ohase is the most relevant in the whole process Im native metric user, and I ve used that approach while manually threading. One should definitly check it every time when working on threads to see if it fits, theres no other way for me at least. 550 rpm worked fine for 1/2 unf thread in aluminium and steel.