Lathe Post Processor?

ecs

ECS
Hi Guys,

What post processor is everyone using for there lathe when using fusion?

Cheers,
Josh
 

gear

Gear
I am using the Fanuc Lathe post processor. Unfortunately you have to edit the tool changes to the format "Tx M06".
 

ecs

ECS
@gear The Fanuc turning one?

Do you change this for every gcode file or is it something you do to the post processor once off?
 

gear

Gear
I am currently editing the code. It can be changed in the post processor but I have not figured out how to do that yet.
 

machinedude

machinedude
if you guys want I can take a look at it and see if I can make the changes to that post processor. you will just need to tell me what needs changed so I can see if I can help you guys out with this.
 

ecs

ECS
@machinedude I'm not sure yet. I ran a little file today and my machine didn't do anything i wanted it to do lol

I've only used the wizards and everything works great with that but when i used the gcode from fusion today nothing went to plan.
 

machinedude

machinedude
@ecs maybe if you use the wizard for something and do a program in fusion to reproduce what you did in the wizard I can compare the two so I can see what I can tweak in the post processer. nothing fancy is needed just some small samples of code form both is what is needed to start with. so something simple that works with the wizard and the same in fusion which is not working is what we are looking for.
 

machinedude

machinedude
I opened up this post and was looking around and it looks like it supports different lathe configurations. so there are some things to set on the post processor that probably are done by checking some boxes for the type of machine you have before you post any code. every post processor is different the ones that are a little more complex give you some options to customize without the need to actually get into the post processor itself. all this is done in the logic within the post processor.
 

ecs

ECS
@machinedude yea i saw this and have been scratching my head about this. There is nothing in fusion to set this up with regards to tool change.

I mean the post has a QCTP option but how do i select that? Maybe it checks this on the Fanuc before running the gcode?
 

ecs

ECS
@machinedude I got it to run a program! It kept stopping on a U0 code. But i think it was stopping because of the tool change (just wasn't stopping at that code on the screen). The post doesn't give the correct code for the tool change.

Its giving the tool change like this.
N14 M0 (CHANGE TO T1 ON REAR TOOL POST)
N15 T0101



When it should be
T1 M06 (for tool 1 example)

Again it also says Rear tool post and i'm not sure how to configure it to a QCTP like in my setup.
 

machinedude

machinedude
a M00 is a program stop you will see that before your tool change that is normal. the m06 is not really doing anything since you have a manual tool change the T1 should have some reference to some offsets for that particular tool so you can continue with your program. that part I am not sure on because I don't have the lathe control to play around with.
 

breezy

Arie
Staff member
Quote from ECS on July 24, 2019, 8:00 am

Again it also says Rear tool post and i'm not sure how to configure it to a QCTP like in my setup.

Looking at the FANUC post processor I noticed this description with shows up when you hover the mouse over the selected post processor in FUSION Post,

"Generic turning post for FANUC. Use the property 'type' to switch the FANUC mode A, B, and C. The default mode is A. Use Turret 0 for Positional Turret, Turret 101 for QCTP on X- Post, Turret 102 for QCTP on X+ Post, Turret 103 for Gang Tooling on X- Post, Turret 104 for Gang Tooling on X+ Tool Post."

About half way down in the property box there is an entry for TYPE which can be changed to A,B,C. But I couldn't find where to change TURRET. Had a quick look in tool library and there is a setup tab in which you set the Orientation in Turret, maybe that's how FUSION tells FANUC which TURRET to use.
Quote from machinedude on July 24, 2019, 8:53 am

a M00 is a program stop you will see that before your tool change that is normal. the m06 is not really doing anything since you have a manual tool change the T1 should have some reference to some offsets for that particular tool so you can continue with your program. that part I am not sure on because I don't have the lathe control to play around with.

The M06 is required on a manual tool change as it causes MASSO to stop, move to tool change position.

My checking of the post processor for tool change it seems to use this bit of code in function onSection()

"writeBlock("T" + toolFormat.format(nextTool.number * 100 + compensationOffset));"

This is where you need to change all the writeBlocks to something like this

writeBlock("T" + toolFormat.format(nextTool.number) );

writeBlock(mFormat.format(6));


This line

"writeBlock(mFormat.format(0), comment);"

and " onCommand(COMMAND_OPTIONAL_STOP);" needs to be commented out.

Hope this helps.

Regards,

Arie.

PS.

I tried that and FUSION didn't like it. It report this

#########################################################################
Error: SyntaxError: missing ) after argument list
Error at line: 780
Failed while processing global script.
###############################################################################​


But I couldn't find missing ) on that line, so I returned the modified lines to original, but retained commented out and extra lines. FUSION was happy and the resultant files produced these results default FANUC

(SINGLE GROOVE4)
M1
T1313
(ISCAR SQUARE PARTING)

modified MASSO

(SINGLE GROOVE4)
T1313
M6
(ISCAR SQUARE PARTING)

Attached modified cps file.
 

Attachments

  • MASSO-turning.zip
    11.3 KB · Views: 17

machinedude

machinedude
@breezy

I guess the M06 has some function after you mentioning the tool change position I stand corrected :) I seen the types A , B, & C and thought that might be something as well but when I looked deeper I was seeing too much inside the post. I did notice the font and back looked like the were reversed in the post processor. I think those control a modal offset in the logic of the code that drives the post processor. I was thinking the front should be the + and the Back should be the - but it looks like it's the other way around inside the post processor. sometimes the answer is in the variable list at the beginning portion of the post process. these things are usually segmented into key groups like beginning , middle and end usually the middle has a lot more going on as far as coding goes.

no doubt these can be a pain in the back side I've had my fair share of frustration with them. if I remember right most of the errors I got were because of a format issue. I think these are done in visual basic?
 

ecs

ECS
@breezy can you screen shot where the tool library setup is? I can't seem to see it on mine.

That edit didn't work completely but it did give me an idea. I went into the Masso mill post processor they have on fusion and found the section on tool data. Found the difference and made the changes and it worked!!!

The tool change screen comes up and the spindle stops. I hit cycle start and then spindle start up. Then it just sits there until i press cycle start again(is that normal to press cycle start twice?)and then it continues.

@machinedude not sure what it is. NYCCNC has some good info on the post processors.
 

testyourdesign

testyourdesign
I followed the post processor modification instructions from Tom in this video to get mill turn function to work with Masso post. Maybe that will help you.

Cheers,Stephen Brown
 

machinedude

machinedude
working with these is just one of those things that you just have to go through a trial and error process until it's sorted out. the company I work for was looking into getting one custom made for the laser they bought a few years back and it was going to cost somewhere around $750 to $1000 just to have one made. so it's worth messing around with them to get them working.

a lot of it boils down to how much modification is needed? sometimes you don't need to change much and it's just a minor tweak other times it's a lot more involved. i'm glad you made some progress with it and glad others jumped in to help out. one of the things I like about this forum are the members willing to jump in and try to help others.
 

breezy

Arie
Staff member
Quote from ECS on July 25, 2019, 7:43 am

@breezy can you screen shot where the tool library setup is? I can't seem to see it on mine.

That edit didn't work completely but it did give me an idea. I went into the Masso mill post processor they have on fusion and found the section on tool data. Found the difference and made the changes and it worked!!!

The tool change screen comes up and the spindle stops. I hit cycle start and then spindle start up. Then it just sits there until i press cycle start again(is that normal to press cycle start twice?)and then it continues.

@machinedude not sure what it is. NYCCNC has some good info on the post processors.

@ecs

I don't use the lathe version (The shed has a CNC Router) but having to press cycle start twice does occur in certain operations on the mill version.

Glad that you sussed out how to charge the post to get it to work.

The tool setup is in the the tool edit dialog.

Regards,

Arie.
 

Attachments

  • Tool-lib-setup.JPG
    Tool-lib-setup.JPG
    112 KB · Views: 16

ecs

ECS
@machinedude Looks like i have everything working now. Couldn't agree more on the help on this forum. Its amazing how when a few people come together the wealth of knowledge is incredible.

@breezy Thanks for that. I totally forgot that was in there. It happen on all the tool changes for the lathe for me. Not a big concern as it gives my lathe time to spin to the correct RPM before starting.

Thanks to everyone again for all your help!!
 

breezy

Arie
Staff member
@ecs

If you have a working MASSO Lathe post, provide it to MASSO Support so they can add it to the Post Processor documentation page.

Regards,

Arie.
 
Top