Machsupport Forum
Mach Discussion => Mach4 General Discussion => Topic started by: Cbyrdtopper on May 01, 2019, 04:43:44 PM
-
I am double checking that we cannot change this "P" Value from the code that Fusion 360 posts.
G1 G41 X-1.683 Y-0.083 P0.0625
As it is, I don't think we can take advantage of cutter comp from Fusion 360 because it posts this P value instead of a D(#).
I'm just clarifying that we can't change this P value anywhere from Mach4.
I feel like Fusion should be posting a D value so all we have to do is change the Tool Diameter or Wear from the tool table and not have to manually change this P inside the program manually.
-
What is that P, Chad? Diameter as defined in Fusion, radius, something else?
Likely we'd need to edit the Fusion post to output the D instead.
In modern times I've gotten away from using cutter comp!! Mach3 didn't do it the Fanuc way, as I remember, and while Mach4 does, I've taken to using stock in the CAM software, measuring, change the stock, repost!! It's either change the cutter comp and rerun, or change the stock in CAM and rerun, not much difference. Back in the punched paper tape days it wasn't so easy to repost as it is now days, so changing cutter comp was easiest. Back in those days I insisted on reading the Gcode and if it was cutting across at Y 1.000 on the print, I wanted to see Y1.000 in the Gcode, dammit, not Y1.246 or something!!! That habit died hard but it's dead now!!
Tom
-
Hey Tom,
From what I noticed it puts in the tool radius as thr P value.
I want to use cutter comp so I don't have to walk back to my computer at work. I usually just put a negative stock to leave, but I want to edit finish passes right from the control.
Once I get home I'm going to edit the post processor to get it to post a D instead. I've got Visual Studio Code on my laptop... So nice for editing post processors.
Still, I think the stock post from Fusion should output the D instead of P.
-
Is it a Mach3 post or a Mach4 post?
Mach3 works with the P(radius).
-
Mach4 post.
The P works, but I want to change the diameter of my tool in the tool table or adjust the wear in the tool table to be able to change the dimension of my part and not have to go into the code to adjust the P.
Autodesk replied to the post on the Fusion forum, they have already fixed this and it will be in the next Post Processor Update.
-
Still, I think the stock post from Fusion should output the D instead of P.
I do, too!! Maybe you can sweet talk them into changing it, like you did with the G30 thing. That was great:)
Tom
-
Straight from the Fusion 360 forum.
"Yes, Autodesk has actually changed this internally. You will see an updated post at some point in the future."
-Seth Madore
Fusion 360 CAM Specialist
So hopefully soon!!
;D ;D ;D
-
For now,
This seems to fix the problem until Autodesk releases the new Post Processor for Mach4.
https://forums.autodesk.com/t5/fusion-360-manufacture/modifying-postprocessor-for-mach4/m-p/8745647?advanced=false&collapse_discussion=true&filter=location&location=category:1234&q=mach4&search_type=thread
Be sure to change the G42 line as well; it is about 4 lines after G41, just repaste the G41 line and change it to G42.
-
Cool! And herein lies one of the problems with customizing stuff. Like the wx4 screenset I've customized, and renamed, of course. If the wx4 screenset changes in the future with something I'd like, I'd have to go into it and figure out all the edits I've made and add them to the new version. I don't know of a way to copy/paste from one screenset to another, is there a way? Mach3 had some third party screen editors that allowed this, but Mach4 screen editing seems to be sticking to the built in editor and no one is doing screens like they did in Mach3, or very few anyway. I guess that's good because Mach4's built in editor is good, the basic screens are good, so people are just using and making the small edits themselves.
Same would hold for the Fusion Mach4 post. I've customized it pretty heavily for my knee tool length action and would have to go in and figure all that out and do it again in the new post!! I guess I'd go into the new post in VS Code and see how they did it and fix it in my post!! Ah, I see we're typing together, I'll check out your link and see if I care to fix it in my post. Thanks.
Tom
-
Tom,
I have made some changes to a Mach4 post as well, future use of a 4th axis brake and such.
An easy way to keep track of changes is to make a text document and make extensive notes on your changes.
Where it was in the Post, Line number (even though that will for sure change) the section it was in, and what specifically was changed.
I do the same with Mach4 screens, only I have a document filled with functions and edits for future projects that I just copy and paste into the respective screen code.
-
I know, I know, I always think about documenting when making changes then don't do it!! I'm good about commenting IN the code, but that doesn't help me find ALL the little edits I've made over the years in the screenset where the code is all over the place :-\ At least in the post it's one chunk of code so sorting thru for my comments is easier than finding them all over in the screen.
I'm going to make Seth's G41/G42 edits to my Fusion post just for the exercise and while I'm in there I'm going to sift thru, find my internal comments, and document them in a separate file for future reference. I don't have nearly as many edits in the post as in my Mach4 screenset!!
Tom
-
To find the differences in 2 screens scripts......... open each in Mach4 and then operator, view screen script, copy all and paste into notepad ++. With both versions of script open in a tab use their compare plugin. Every difference (no matter how small) will be made obvious.