topic Re: Post programe in Fusion Manufacture Forum

Post programe

Anonymous — Mon, 04 Apr 2016 03:33:21 GMT

Curently using Enroute for machine gcode and tooling is there an easy way to find the correct post code from fusion to my machine without just trying all the types?

Re: Post programe

Anonymous — Mon, 04 Apr 2016 12:21:10 GMT

Hi, @Anonymous!

I've just moved from EnRoute to Fusion (we have Multi-Cam machines.)

What kind of machine do you have? I can help with the transition, definitely.

Re: Post programe

Anonymous — Mon, 04 Apr 2016 20:58:37 GMT

We have an Australian built Multicam running Enroute. I am just looking for the best processer to use instead of running through all the different types Fusion has to find one that works.

Re: Post programe

Anonymous — Tue, 05 Apr 2016 11:32:00 GMT

The standard "MultiCam" Post that comes with Fusion should work fine for you then. It worked on our machines.

If you need to make some changes, let me know and I will help you out - I had to alter our post for some things, so I'm familiar with the Post Processor.

Run some air cuts, or even better, grab an old file and redo the cnc in fusion. Compare the g-code for the two of them (or post the old and new file here and I can take a look). That will be the easiest way to see if it will behave the way you expect.

Thanks, and good luck!

Re: Post programe

Anonymous — Tue, 05 Apr 2016 21:19:35 GMT

Hi Autumn S thaks for the reply! I am curently teaching myself the basics of Gcode and the functions of them on my machine.

I looked at the posting options for Multicam and the only 2 I have acess to have .PLT and .CNC where as our machine uses .NC ?

I have attached a section of post from Enroute to the format our macine accepts.

All so I seem to be getting -Z values in Fusion on the posts and have attached a screen shot of the orientation. I know it must be something simple I am missing but being new to the 3d space setup I have not grasped the concept of orientation I think.

Re: Post programe

Anonymous — Wed, 06 Apr 2016 11:53:17 GMT

Hi @Anonymous,

Hmm, this may need to be taken to the autodesk CAM forum, then. I've never used .nc files for my Multicam - and in fact, mine doesn't support .nc file types as far as I know.

As for the negative, you can choose whether to design in negative z-space or positive z-space. It all depends on how you set up your Post and WCS. Mine is set up to work in neg. (My Enroute was in Neg. Z as well).

Go ahead and repost in the CAM forum here : http://forums.autodesk.com/t5/post-processors/bd-p/218

Include the information you've given me here. I'm sure they can help you.

Sorry I couldn't help!

Re: Post programe

Anonymous — Wed, 06 Apr 2016 13:28:06 GMT

Actually, I took a stab at it and think I got it figured out, @Anonymous.

I changed "Filetype" to nc and changed the zFormat line from -1 to 1.

I attached the updated post here.

Mke sure you DO NOT put it in the regular "post" fole for fusion - that folder moves every update. Create a personal post folder or use A360 Drive and enable cloud posts in your preferences.

This will work with your current WCS setup you poosted earlier as well.

Run a Post using this, and if you need more of the code changed, let me know.

Re: Post programe

jeff.walters — Wed, 06 Apr 2016 13:29:35 GMT

The .CNC and .NC are simply file extensions they don’t effect the code format. The file its self is just a text file. The only reason for different extensions is simply what the control is set to look for. First question have you tried putting the .CNC file in the machine? If it doesn’t like it try changing the .CNC to .NC and see if it works. If it does than it’s a simple post change to have the extension set to .NC automatically.

Re: Post programe

Anonymous — Wed, 06 Apr 2016 13:40:22 GMT

Hi @jeff.walters,

Yeah, I realized that right after I posted - never answer questions before you're awake, is the lesson I learned!

I attached him a post above changing the extention to .nc and setting the z in positive space. I hope it works for him!

That is always the biggest wake-up to most Multi-Cam users - Enroute (the old CNC program that Multicam recommends) defualts to working in positive Z, but the Multicam Post in Fusion defaults to negative.

I get the feeling this may come up a lot as Multicam users switch.

Re: Post programe

Anonymous — Wed, 06 Apr 2016 21:27:01 GMT

Wow thats looks a little complex!! haha So before you loose me I will ask how to use the file you attached.?

Ok my understanding is your file is a posting paramiter file ? eg I save this safely and then when I go to post toolpaths I select this file as my Post Config file?

I will try this when I can as I havent been in the shop much but I thought better to ask first.

And thank you so much for all the support, it is great to find a programe with large community of supporters!

Re: Post programe

Anonymous — Fri, 08 Apr 2016 05:58:46 GMT

Ok still have not run on the machine yet but posted a toolpath through the cps file you provided and still got a negitive value?

Re: Post programe

HughesTooling — Fri, 08 Apr 2016 08:42:56 GMT

Can you export your Fusion design and attach to this thread, from the file menu pick export set file type to F3D pick a folder under Save to my computer. There's something odd, looking at your screen shot it should work so we need the file.

Mark

Re: Post programe

Anonymous — Fri, 08 Apr 2016 23:35:32 GMT

Ok so I have 2 f3d files I will attach, the same layouts an extruded box with a extruded hole cut through.

Now strangely the one file with no neg z post problems was an auto backup file that i pulled up and ran through the new post processer,

and the file with the neg value i built and ran throught the new post processer just prior to writing this.

All origin and tool locations are at the same points so not to shure why a previous auto save would be ok and a new part would not?

Could it be to do with being an Untitled part? as I am just building it then straight to cam without saving or specifying job details.

Re: Post programe

HughesTooling — Sat, 09 Apr 2016 09:02:56 GMT

Took me a while to spot what was wrong. In the op you've enables Tool Orientation, this is for 4 and 5 axis machining not to set the origin for 3 axis, you set the origin in the setup and that's it, leave Tool Orientation unselected.

When you post the setup origin is used.

Mark

Re: Post programe

Anonymous — Sun, 10 Apr 2016 22:52:52 GMT

Hello there I finally had some time to send a post to the machine and it came back with some errors.

We have an A2MC File manager as the controller on the machine and it reported

No NC Number E214

Bad G2/G3/R code A E207

I have attached the 2 nc text files 1 from Enroute and 1 from fusion.

I will try some of the other post processers to see if any others work latter today.

Re: Post programe

HughesTooling — Mon, 11 Apr 2016 09:40:31 GMT

Looking at files there seems to be a couple of differences.

One comments from Enroute start with ( and from fusion start with //

Two it looks like circle centres are ABS from Enroute and incrimental from Fusion. Something else that might be a problem is does your machine support none XY arcs. Do you have any info on supported G codes does it support G18 and G19.

Anyway I modified your post to ABS circle centers see it that helps.

Mark

Edit just notices a line G74 that should put the control in to incremental IJK, I updated the file and removed the G74, give that a go. If you still have a problem it could be down to the G18/19.

Re: Post programe

HughesTooling — Mon, 11 Apr 2016 09:46:37 GMT

Just noticed the Enroute code has a G56 offset called, from what I can see the MutiCAM post doesn't support work offsets, will you need them?

Mark

Re: Post programe

HughesTooling — Mon, 11 Apr 2016 12:14:18 GMT

@Anonymous do you have any info on supported G codes. Looking at the g code from the post I modified it takes the machine to Z0. at tool changes, normally you have a G28 or G53 on that line. In the post it's using a machine configuration to set the tool change position but I don't think they're supported by Fusion yet so the post will need another mod for that.

Mark

Re: Post programe

Anonymous — Mon, 11 Apr 2016 12:31:05 GMT

Hey guys...Sorry I dropped off the map, I got sick.

I have attached my (fully) modified post for my mulitcam. This may just be confusiong things further, sorry.

This post has ben running and working on our machines (we have 3) since December.

I did comment out quite a lot (like the comments on tool type etc) and added a "return to back" at the end of cycle.

Hopefully this helps you guys understand better. I think @Anonymous has a machine with quite a few more restrictions than mine.

Re: Post programe

Anonymous — Mon, 11 Apr 2016 22:02:14 GMT

Hi again VERY excited I found a generic fusion post the runs my machine and cut some 3d contoured faces into foam yesterday it was the opticut.cps generic.

This has no tool changeing but the code outputs to the machine!!!

I ran your post process and the I and J values have to be whole numbers for it to work but ther is still a G0 Z0 move that would crash the machine at start and finish I will attach the txt files.

I also ran a Generic NUM test it had sucsess in the machine but had a G0 Z0 at the start and finish of the cycle.

Multicam Australia run a different A2CM controller software from what I have found out and are not much help when it comes to questions about other programes they do not sell.?

Thank you again for the help looking at this problem and I know a few people that run these machines in Australia that would be very interested in a post programe that functions with Fusion!