Why would Fusion 360 be adding an unwanted G10 line to my post?

Been Googling and searching and can't find the answer so figured I would ask here.

My post's for Fusion 360 add a G10 line near the start of the program after which it doesn't actually seem to do anything but about 50 lines of code scroll by at the first tool change. I am guessing it is a macro since it has program structure.

Anyhow, first time it did this I ignored it and doing a single block watched it drop a 2" face mill 1.5" under the Z surface. Thank god no stock loaded as it was a first test. It hadn't done that in the simulation before I ran the post so needless to say the almost huge crash had me a bit startled. I checked the Offsets page on the controller (Fanuc 0i D) and the tool offset had been cut in half from what I had just preset it with the Renishaw presetter. Needless to say I was startled to find this change.

Short fix was just deleting the G10 line. After that it still runs some macro that I am not putting in the program on the first toolchange (and any toolchange after that even if I am in MDI with no program running until the controller is restarted) but it doesn't seem to effect anything.

How do I get Fusion 360 to stop putting in this G10 line and triggering whatever that macro is? I found the Tool Offset WPS in a post setup dialog box, I think it was for Stock. But it is set to 0, as was the Work Offset one above it. Not an on/off checkbox.

How do I get it to stop putting this line in? Getting sick of deleting it everytime I post something new.

Thanks guys.

Try opening the post with a text editor and search for G10. You should be able to find the line(s) where G10 gets inserted, and simply comment it out. Test and retest before putting into production.

rklopp said:

Try opening the post with a text editor and search for G10. You should be able to find the line(s) where G10 gets inserted, and simply comment it out. Test and retest before putting into production.

Click to expand...

Fusion 360 opens an editor when it is done Post. It's called like Brackets or something. I have just been deleting the line every time. The program runs fine after that except for that strange macro thing on toolchanges.

I was just wondering if there was a way to get it to stop putting it in in the first place. I just assume I have some setting wrong in Fusion 360 so it is trying to allow it to set my tool offsets with the program which for obvious reasons I really don't want it doing since it was putting in incorrect values.

As I said I thought I found something in the Stock dialog box about WCS and Tool offset changes being allowed by Fusion 360. Haven't found it since then. Looking now.

Edit the post processor to keep it from inserting the unwanted code. As I remember it isn't terribly difficult. YouTube has videos and you can find plenty of help on the Fusion forum.

Sent from my SAMSUNG-SM-G890A using Tapatalk

Jaxian said:

Fusion 360 opens an editor when it is done Post. It's called like Brackets or something. I have just been deleting the line every time. The program runs fine after that except for that strange macro thing on toolchanges.

I was just wondering if there was a way to get it to stop putting it in in the first place. I just assume I have some setting wrong in Fusion 360 so it is trying to allow it to set my tool offsets with the program which for obvious reasons I really don't want it doing since it was putting in incorrect values.

As I said I thought I found something in the Stock dialog box about WCS and Tool offset changes being allowed by Fusion 360. Haven't found it since then. Looking now.

Click to expand...

I meant the post processor Javascript code or whatever that code is, not the G-code. Rescue35 to the rescue! On my Mac, the custom posts are in Users/<my username>/Autodesk/Fusion 360 CAM. The default posts are buried. The F360 forum explains where they are. You can copy from the default posts folder over to the custom posts folder, and then edit the post.

Before going any further, what post are you using?

BTW have you asked this question on the Fusion CAM forum (or the Autodesk HSM forum - subforum=post processors)? Not saying you won't get an answer here, but might get a quicker reply there.

As others have mentioned, you need to open up the post (the xxx.cps file) in an editor - Brackets or any text editor - and amend it to remove/comment out the G10 or the logic that is creating this code and the presumed macro.

Fred

Freds said:

Before going any further, what post are you using?
Fred

Click to expand...

Right now the post I am using was the one for Doosan 3-axis VMC from the Autodesk Fusion 360 post list on Autodesk website. The information thing said I think it was written by Autodesk, although I recall there was a "you better check it" warning.

Oddly the file was just called doosan, it had no file extension until I added it. Then it worked fine. Not sure if that is standard procedure so just went with it.

Machine is Doosan DNM5700

EDIT: I need to find out what the best Fusion 360 forum is so I can join up and see what information is there. There is just so much Fusion 360 information out there it is kind of hard to figure out what is what.

Hopefully the one by Autodesk itself is the best as it's the easiest to find. Lots of times that is not the case with software companies as they tend to be WAY over moderated to keep constant discussion of bugs and negative comments low.

Just took a look at the Doosan VMC post. The option for entering tool lengths via G10 is set to true; needs to be changed to false. Pull the post file up in a text editor and go to line 52 (as numbered by the editor) and change to 'Use tool length option' to false. Hopefully that should take care of the problem. I believe it is telling the program to insert the length of the tool from the tool description and substituting it for the actual tool length offset.

I think the Autodesk HSM Forum/sub forum Post Processor may be the best option, but you can also look at the Fusion website and go to the Fusion Forum, then CAM to ask any questions as well.

Fred

Freds said:

Just took a look at the Doosan VMC post. The option for entering tool lengths via G10 is set to true; needs to be changed to false. Pull the post file up in a text editor and go to line 52 (as numbered by the editor) and change to 'Use tool length option' to false. Hopefully that should take care of the problem. I believe it is telling the program to insert the length of the tool from the tool description and substituting it for the actual tool length offset.

I think the Autodesk HSM Forum/sub forum Post Processor may be the best option, but you can also look at the Fusion website and go to the Fusion Forum, then CAM to ask any questions as well.

Fred

Click to expand...

Thanks a ton Fred. I will try that first thing tomorrow morning. Fantastic!

Paul B.

After posting my remarks, took a second look. I tend to modify the post files (.cps) and make all my changes there. However, in the case of 'writeToolLength' (the option that is causing the output of G10) you can actually change it when you post. Go the the Post Options section of the posting dialog and scroll down to the bottom where you will find it set to 'Yes' and change to 'No' - this will accomplish the same aim without having to open up the post.

Having said that, it is not obvious from just looking at the Post Options in the dialog that this was/is the culprit - you could only really see this when you actually looked at the .cps file in an editor.

Fred

Just did a post on a new program with your change Fred and bingo no G10 in the post. Thanks a ton man.Going to go out and run a part shortly and see how it works.

Unfortunately have to re calibrate my Renishaw presetter as it's having some issues with not working in manual mode with the Doosan EOP and the automatic mode is a bit rough. As in a 2" facemill hit the side of the presetter touch point and since it was running in reverse kind of impact wrenched the touch arm loose. I tightened it back down but now my tool offsets aren't going in on size. Never re-calibrated one of these but Doosan has a section in their manual on doing it using their EOP interface for the Renishaw. So hopefully can get that sorted and test it out.