EMCO Mill Post Processor

[Anonymous]

I help manage Reynoldsburg Battelle FabLab and we have an EMCO Concept Mill 55 and an EMCO Concept Turn (CNC Lathe).

I would like to get a post for Fusion 360 that will work with these machines.  I have tried the generic post but get multiple errors.

I have contacted our EMCO agent and he is willing to work with AutoCad to create a post.

Does anyone already have a post?

or

Solution suggestion?

or 

Contact info to AutoDesk?

I have been unable to find a solution on the support site.

Any help would be greatly appreciated!

[Anonymous]

Hello from Greece

my name Vaios Pontikas

I have in my possession relatively recently one emco concept mill 55 

(EMCO WinNC for Sinumerik Operate Mill Software description software version from 01.04)

http://www.emco-world.com/uploads/tx_commerce/EMCO_WinNC_for_Sinumerik_Operate_Mill_EN_1848_C_02.pdf

I am at an initial stage of training Sinumerik Operate Mill Software but also in Fusion 360

I tried to use it post post processor sinumerik 840d but I did not succeed

You think I will need somebody else post processor Specialized for this machine(emco concept mill 55) ?

I make some mistakes

thanks vaios

[Anonymous]

Hello!  I just picked up a PC Turn 55, basically Identical to the one you have written a lathe post for.  Also has Fanuc 21.  I am wondering if you finished modifying this post for the lathe?  I did use the first one but yea had G50 issues.  I will be as absolutely helpful as possible, however I am new to G code.  I can do quite a bit with fusion CAM/CAD, however and have been using it for my Bridgeport over the last year.  

[LibertyMachine]

Tsk. I saw this post come across my email but I was up to my eyeballs in craziness. My work has taken a turn for the crazy lately....

The last reply from the OP was made the same week I quit my day job to work for myself full time. I think it's understandable that I didn't quite get to it, and then it got forgotten. I will play with the post today and get those final bugs sorted out

[Anonymous]

Hello!

So I have been able to mess around some with the Emco lathe and post you have made.  Here is what I have found out so far.  Threading does not work.  I have only tried OD threading and have realized that there seems to be no G codes that should let it know it is trying to thread.  (From my limited knowledge)

EMCO post, Fanuc "A"

N1 G40 G70 G80 G90

N2 G95 G96 G98

N3 G50 S4000

N5 G28 U0.

N6 T0606 M9 (OD THREADING)

N7 G97 S100 M3

N8 G0 X1.4275 Z0.2366

N9 G0 Z0.4955

N10 G1 X0.5875 F39.37008

N11 Z-0.8903

N12 X0.7169 Z-0.955

N13 G0 X1.4275

N14 Z0.4911

N15 G1 X0.5719 F39.37008

Now about the G50 issue, when I change the EMCO post in the program settings when I post it out from Fanuc "A" to Fanuc "C" The G50 is gone and it goes to a G92, which appears appropriate for Fanuc "C" codes.

To preface, it appears that EMCO fanuc 21 Lathe is using Fanuc "C" per their manual.  I am attaching that EMCO document as well as a FANUC/EMCO document that outlines this version of code.

Here is where It gets confusing to me; I posted the same code each with :

Emco Fanuc A

Emco Fanuc C

Generic Fanuc turning A

Generic Fanuc turning C

Generic Fanuc "C" appears to me the most consistent with what I possibly need.  It has the G92 (instead of G50, a fanuc "A" code).  It also has a threading G32.  However in the highlighted area on page 21 of the EMCO CT55 reference, G32 is an "A" category code, and G33 should be the "C" category code.

 Note: The lathe must need "C" codes, as it will error out on G32, it runs G33 however.

In that same CT55 reference it shows their threading on a canned cycle of G78.  So what is best for CAM, a G33, or G78, or G21?

Also G28 U0. seems to error out.  Program seems to function if I delete the whole line, though not sure if I need a return to reference point? 

This is all the farther I have gotten... please advise if you want me to test anything, I hope this helps in starting to edit this post.  Let me know. Thank you!

[Anonymous]

O4003 
N10 G90 G95 G18 
N11 G20 
N12 G92 S4000 
( THREAD3 ) 
N14 T0606 
N15 G54 
N16 G94 
N17 G97 S0100 M3 
N18 G0 X1.4275 Z0.2366 
N19 G0 Z0.4955 
N20 G1 X0.5875 F39.37008 
N21 G33 Z-0.8903 F0.090909 
N22 X0.7169 Z-0.955 F0.090909 
N23 G0 X1.4275 
N24 Z0.4911 
N25 G1 X0.5719 F39.37008 
N26 G33 Z-0.8869 F0.090909 
N27 X0.7169 Z-0.9594 F0.090909 
N28 G0 X1.4275 
N29 Z0.4877 
N30 G1 X0.56 F39.37008 
N31 G33 Z-0.8843 F0.090909 
N32 X0.7169 Z-0.9628 F0.090909 
N33 G0 X1.4275 
N34 Z0.4849 
N35 G1 X0.5499 F39.37008 
N36 G33 Z-0.8822 F0.090909 
N37 X0.7169 Z-0.9656 F0.090909 
N38 G0 X1.4275 
N39 Z0.4824 
N40 G1 X0.5411 F39.37008 
N41 G33 Z-0.8802 F0.090909 
N42 X0.7169 Z-0.9682 F0.090909 
N43 G0 X1.4275 
N44 Z0.4801 
N45 G1 X0.5331 F39.37008 
N46 G33 Z-0.8785 F0.090909 
N47 X0.7169 Z-0.9704 F0.090909 
N48 G0 X1.4275 
N49 Z0.478 
N50 G1 X0.5257 F39.37008 
N51 G33 Z-0.8769 F0.090909 
N52 X0.7169 Z-0.9725 F0.090909 
N53 G0 X1.4275 
N54 Z0.4761 
N55 G1 X0.5189 F39.37008 
N56 G33 Z-0.8754 F0.090909 
N57 X0.7169 Z-0.9744 F0.090909 
N58 G0 X1.4275 
N59 Z0.4742 
N60 G1 X0.5124 F39.37008 
N61 G33 Z-0.874 F0.090909 
N62 X0.7169 Z-0.9763 F0.090909 
N63 G0 X1.4275 
N64 Z0.4725 
N65 G1 X0.5063 F39.37008 
N66 G33 Z-0.8727 F0.090909 
N67 X0.7169 Z-0.978 F0.090909 
N68 G0 X1.4275 
N69 Z0.4709 
N70 G1 X0.5005 F39.37008 
N71 G33 Z-0.8714 F0.090909 
N72 X0.7169 Z-0.9796 F0.090909 
N73 G0 X1.4275 
N74 Z0.4693 
N75 G1 X0.495 F39.37008 
N76 G33 Z-0.8702 F0.090909 
N77 X0.7169 Z-0.9812 F0.090909 
N78 G0 X1.4275 
N79 Z0.2366 

N80 G28 U0. W0. 
N81 M30 
% 

Also getting a "6014 NO SPEED FOR MAIN SPINDLE" alarm when I run the above code, (Which I manually changed the G32's to G33, and deleted the initial G28).  Not sure what that is about as it has clearly shown a spindle speed of 100.  

[redcapjuice]

First off, I'd like acknowledge the age of this post. I know it's old, however it's helped me tremendously! 

I have been able to get my concept mill 55 up and running with the post in here, with a couple edits.

The post as is does work, but you need to remove the .nc file extension when saving. Also, each file needs to be renamed in the editor to start with an "o". I use a capital o, not sure if it matters, but I used a lower case here as not to confuse anyone with a zero. The last thing I had to figure out was I have to remove the % from the first line, and start the program with the program make on the first line. 

In the grand scheme of things, these are super minor. I would love to get the post to the point where I don't need to rename and edit every time, but it works enough.

I do however have another issue with this post. Jerky circles. 

Here is a video of me doing a "bore" operation. At 2:00 in the video you can clearly see the issue.

https://youtu.be/WbrK12B_GJo

I also had this issue with using other operations on round holes or profiles.

The circles come out round, however it's just not right. 

I have not messed with the smoothing or tolerance settings yet, as I'm still very new to all of this. But it seems like the machine is just doing chunks of an arc at a time.

My hope is to work through this issue in this thread, as it was the first thing to pop up on a Google search. I feel it would be great to have a polished working post right here, instead of info scattered about.

[Steinwerks]

The pausing nature of the toolpath is likely due to the machine and not the post, but if you want to share that part file (exported as .F3D) and the post you're using right now I can take a look. There may be an acceleration setting in the machine like G08 that allows for smoother motion (Fanuc and Fadal used to use this, Fanuc has made it more granular as an option and most controls have similar features).

[redcapjuice]

Attached is the file in the video above, as well as the post I used. 

In this post, I already removed the .nc file extension, but cannot find the part to remove the % at the beginning of the program. 

Also, is there a way to allow me to save the program when posting as O1111 vs 1111? Whenever I try to I get an error and the program will not post. 

Thanks! 

[LibertyMachine]

Ahh yes, I remember this post, I think it was one of my more involved edits. I enjoyed working on this one, glad it's still helping people out.

The changes you are looking for should be doable, give me the afternoon to pick away at it as I have time

I think your choppiness might go away if we allow no more than 90 degrees of arc, breaking the circle up into quadrants. It may perform better with R moves instead of I/J, and that is something we can try later

For the removal of ".nc", is there another extension preferred?

[redcapjuice]

Thanks again for this post as is Seth. It got me going. 

I was able to remove the file extension in the post myself, and is in the version I posted just above. These machines prefer no extension at all. Other than that, I'm kind of lost as to where to go from there.

I have been dying to try single point thread milling, and am not super confident I'll have the best results with the way this chops. 

I will say that the Z feed looks smooth still, during the operation if that helps give any clues towards a solution. 

[LibertyMachine]

Give this post a shot. Changes made:

Removed the "%" from the beginning of file,

Allowed for alphanumeric file naming,

Limited Arc moves to 90 degree sweep,

Changed arc moves to using "R" rather than I/J

I'd like to see if the last two have any effect on the motion of the machine. 

Is the file you attached the one you actually ran in the video? F28. might be a bit fast for your machine, given the cutter vs. feature size

[redcapjuice]

Another leap in the right direction! 
I am now able to post directly from fusion without needing to edit the file! 

The downside is the circle routine still acts the same. 
Also, the file name and comment is missing from the first line of the code. All that needed to be removed from the old code was the % at the start, but the "O1001 (Example File Name)" was ok. 

As for the feeds/speeds for features, I'm still learning some of that stuff. I'm reading a ton, and soaking up as much as possible, but it's a learning process. My main focus is to get the machine hardware and software 100% so I can focus on my own skills. I would expect that if I slowed down my feed, this problem would still be occurring, just slower. 

[Steinwerks]

Do you have a manual for the machine control? Can you try adding a G08 before the circular path and see if it does anything?

Is this running WINCNC?

[LibertyMachine]

One other thing I'd like to determine; Does it still do it on 2D Circular moves? In your video, it's doing it while all three axis are moving. What if it's just moving in the X and Y plane, what then? Try a 2D Circular, cutting above the part so nothing bad happens. How's the motion?

[redcapjuice]

Neal- Yes, I'm running through WinNC, fanuc series 21.
As for the G8, I honestly do not know how to implement it.

Attached is my user manual for my specific WINNC/Fanuc series 21 that I'm using.

Seth- yes this still happens on 2d paths.
If you skip to 10:45 in this video https://youtu.be/_rZsgYFFvRk you can see it clear as day. It gets worse as the diameter gets larger. I was using 2d adaptive clearing here.

I'd also like to take a moment and thank everyone who's contributing here! You guys are awesome and I thank you for your time.

[redcapjuice]

I've been just dealing with the jerky motion until I ran into a problem when my code lines were too highly numbered. I don't remember the exact number, but say it was 10000. That's when I switched the skip lines from five to two. (2, 4, 6, 8 vs 5 10 15 20...)

I haven't noticed the problem since. I also have been avoiding the toolpaths that typically create the problem, however I usually would still run across the issue occasionally. I just realized it's been a month or so since I've last seen it and it was around the time I made that switch. 

Incase anyone experiences this issue in the future, try changing your skip lines .

[Fablab_Manager]

Hi I'm wondering if anyone has improved on the EMCO Concept Mill 55 post processor since 2018? A buddy of mine is writing g-code manually for his machine and I wanted to get him setup with Fusion CAM.

[CNC_Lee]

  @Fablab_Manager 

If the post processor above is still not providing the required output necessary, I offer post processor development services and happy to work out a solution for your friend's machine! Message me if I can be of any assistance.