Post Processor will not work properly in recent updates

[Anonymous]

I just got the hang of Fusion 360 in December, I realized I had a couple updates pending. After I updated, I post processed my project and took my G-code to my CNC for milling, I clicked play and my router went straight down as far as it could into my aluminum CNC Table. The code should have lifted the router 10mm above my material then gone for the first cutting sequence. I have tried playing old G-codes I made before the updates and they went fine. I think it was the updates that messed something up for me. My simulations go perfect, it only goes rouge when I start the carve on my CNC. it is UGS GRBL format. Please help me. 

[seth.madore]

Oh no! When you post the code, do you toggle this:

 

[Anonymous]

@Anonymous 

A tip, if you still have your PP in the "Installed Library" then it is likely getting overwritten by the updates, have a look in your preferences as in the image below  and check that you don`t have the "Automatic Post and Machines" updates enabled as shown below. You should have your PP in either your Local Library or a Cloud Library anyway but if you can`t/don`t want to then look in your preferences to turn the Auto updates off

[Anonymous]

okay yes, I have my PP in my local library now. But when I try to create my .nc file, I click ok to the post process tab and it directs me to my text edit on Mac. I check the code, save it and drag it to my CNC USB to take to the machining computer. When I am in the USB my file named "here we go" doesn't have .nc on the end of it like the others and I dont know how to get it to convert to one. fusion 360 used to just do it. I just says its a unix executable file. 

[johnswetz1982]

Can you just click once to rename the file then type ".NC" at the end? You can on Windows not sure how Macs work...

[Anonymous · Accepted solution]

@Anonymous 

When you are saving out from your Text Editor you may well be saving the file as a native format of your Text Editor ie a "unix" format

When you go to the Post Process point what dialog box do you get appearing, or are you on "NC Program" processing?

Whichever it is you should have a box that you use to set the location that the .nc file is saved to regardless of whether you have the Text Editor showing the code.

What is the location that you have in that box, can you show an image of that, it should be a folder somewhere on your computer where the file is automatically saved to as a .nc file, that is where you should be getting the file from, not the Text Editor.

[Anonymous]

Back up and Milling! Thank you @seth.madore @johnswetz1982 @Anonymous I really appreciate all the advice. I ended up doing a NC program for the first time and processing there vs. going to actions and post processing there. Sure enough I was a .nc file instantly I did not have to go through text edit like I would usually. I also went though some soft limit modifying on my CNC. I am new and still learning so keep a look out for me because I WILL be back with more questions! haha

[seth.madore]

Glad you were able to get up and running. Don't be afraid to ask any Fusion CAM question, we're all glad to help others in the community 🙂

[cassanovaw]

Not necessarily related to the solved problem...But.

I use Fusion 360 and I love it...I have a Camaster Stinger II with FTC and most if not of all the toolpaths work as expected...

One annoyance I have is when the tool-change is requested, the CNC head never returns to X0Y0 and I basically have to crawl over the table to the position where the last tool path stopped...Ideally the last tool path or something just after should return the CNC head to my original X0Y0 to allow me to easily switch the tool.

[seth.madore]

As a general tip, if the issue isn't generally related to the problem originally discussed in the thread, it's usually best to create a new thread. This allows for other users to better search for that same issue 🙂

In your issue, what exactly do you want your machine to do that it's NOT doing?

[cassanovaw]

In my case...Let's make some assumptions:

My CNC bed is 39" wide in the X-direction and 48" in the Y-direction.

My X0Y0 is lower left.

My CNC router has an FTC ( Fast-Tool-Change ) vs. an ATC ( Automatic-Tool-Change ).  Meaning I still have to manually change the bits but at least the X0Y0Z0 have already been predetermined.

The first toolpath completes and its last part engagement is in the upper right which is 14 inches in the X direction and 15 inches in the Y direction.  The tool completes it's work and lifts as it should but then stays in the same X and Y position which means I have to potentially crawl over dust-collectors and various things in my small shop to change to the next operation which entails a smaller bit.  If it would have returned to my original X0Y0 I could have easily make the tool change operation.....Ideally the router head should return to X0Y0 where it is easily accessible.

Let's assume now that I have a really large CNC router such as something like a 6' x 12' such as one of these:

https://www.camaster.com/cnc-routers/cobra-elite-series/ that I did not get the automatic tool change option.  To make a tool change I would literally have to crawl across the table, make the tool change and then run the next operation...

This is not a problem with Fusion 360 at all...It's more an issue with the post-processor that should insert a "return to home" after each operation is done to make it easier for the operator to make a change.

[engineguy]

@cassanovaw 

What is the Post Processor, can you upload a copy of it for checking.

It is pretty easy to make the machine return to the Home position if that is where you would like it to go to but there are different ways to do it depending on the PP.

[cassanovaw]

It appears there is a new one out there at:
https://cam.autodesk.com/posts/post.php?name=camaster%20wincnc

If it works I will post an update. The one I was using is attached below.

[engineguy]

@cassanovaw 

Are you looking for something like the code below where it finishes the Operation lifts up to the Z clearance height, then goes to the Z0 position and then goes to the X0Y0 position, usually the safest route going to the Z0 position before moving in the X/Y directions, see below.

N384 G80
N386 G0 Z20.
N388 G53 G0 Z0
N390 G53 G0 X0 Y0
[Drill M6.8 Through]
[T68 drill DIAMETER = 6.8 ]
N392 T68
[6.8mm SUS Drill (Stubby)]
N394 S3000
N396 M3

If the new PP doesn`t work then using your text Editor go to the section in the PP shown in the image below and change it to what is in the image and you will get the code shown above after each Operation where a tool change is required and also at the start and end of the program. Hope that helps.

[cassanovaw]

Let me give that a try after attempting with the newest Camaster PP.

[cassanovaw]

I have your suggestion a try after realizing that the lastest PP did not do the trick...

Looking at the resulting G-Code I can see:

N14 G53 G0 Z0
N16 G53 G0 X0 Y0

Which I think matches what it is supposed to be doing:

if (words.length > 0) {
  switch (method) {
  case "G28":
      writeBlock(gFormat.format(28));
      break;
   case "G53":
      writeBlock(gFormat.format(53),gFormat.format(0),"Z0");
      writeBlock(gFormat.format(53),gFormat.format(0),"X0","Y0");
      break;
   default:
      error(localize("Unsupported safe position method."));
      return;
  }
}

When I run the program the error in wincnc I get on line N14 that says:

Error - Multiple Commands

Could this mean my wincnc version does not support this syntax?  If so I would assume 

I could modify this a bit and use:

      writeBlock(gFormat.format(53),gFormat.format(0),"Z0");

      writeBlock(gFormat.format(53),gFormat.format(0),"X0");

      writeBlock(gFormat.format(53),gFormat.format(0),"Y0");

[engineguy]

@cassanovaw 

Yes, that is possible, or it may be that after the first G53 G0 Z0 it only needs the X0 Y0 on the next line as it has already "seen" the G53 G0 syntax.

Just a guess, worth a try ??