Gcode Issue...I think

Discussion/questions about software used with your CNC Shark and programming issues

Moderators: al wolford, sbk, Bob, Kayvon

Post Reply
asever
Posts: 34
Joined: Fri Sep 03, 2010 12:17 pm

Gcode Issue...I think

Post by asever »

I am experiencing random rounding over of corners.

I am using Aspire 10.512 with the latest postprocessor (this is a metric project so I am using the metric PP...but I tried it with inches and it did the same thing) I am trying to create a dovetail project. For a machine I have an a CnC Shark Pro Plus HD 25x25x7 and using Control Panel 2. In Aspire I have sharp external corners selected and am trying to cut a simple external profile path. There are no open vectors and no duplicate vectors.

Here is an image showing a close up of the tool path.
https://www.dropbox.com/s/fc4pem0k2jab2 ... 2.JPG?dl=0

Link showing preview in Aspire:
https://www.dropbox.com/s/cxilnksclnumm ... e.JPG?dl=0

Link showing preview in Control Panel:
https://www.dropbox.com/s/e35ax3fb0kwoo ... l.JPG?dl=0

All the above show nice sharp corners.

When I go to cut It looks like this:
https://www.dropbox.com/s/suwafzeipl2il ... .JPEG?dl=0

Lastly here is a copy of the gcode file:
https://www.dropbox.com/s/xwqc6mhsnwbaa ... t.tap?dl=0

Your help is appreciated!
Andy

Rando
Posts: 757
Joined: Tue Jan 06, 2015 3:24 pm
Location: Boise, ID
Contact:

Re: Gcode Issue...I think

Post by Rando »

Asever:

Very likely it's the G64 setting in the preamble. The below image is from a backplotter, showing what the GCode says
to do. You'll notice no rounding-off here either. So, it has to be how the controller is interpreting the code.
Screenshot 2020-12-28 093200.png
That's the "absolute stop" setting, telling the system how close it must come to the specific coordinates in the GCode.
When set to ZERO, the system comes to a complete stop at each ending coordinate before moving on. Higher
values allow it to approximate and smooth it's movements. The Vectric/NWA default when I got my machine was 0.1"!
With a number of 0.1, it will round off corners as it moves, believing it's okay as long as it's within a tenth of an inch.

For me, it would come out of a deep pocket and gouge the top-edge as it came out. :cry:

For precision metalwork, I use G64 P0.001
For wood and stuff, I'd go with G64 P0.005

Looking at your Gcode, it doesn't even specify one. So, I'd add the G64 line in the post right after the G90 Absolute Mode
block. Of course, use metric values for the P field, as it appears you're using them.

That needs to be changed in the post-processor files. Don't worry....that was one of the first changes to the post I made.
Just remember: there are potentially more than one of those G64 entries in the post file.

And, feel free to reply here if you're not familiar with the details of that process; it's not at all difficult. The hardest
part is finding where Vectric stores the things.

Hope that helps,

Rando
=====================================================
ThomR.com Creative tools and photographic art
A proud member of the Pacific Northwest CNC Club (now on Facebook)

asever
Posts: 34
Joined: Fri Sep 03, 2010 12:17 pm

Re: Gcode Issue...I think

Post by asever »

Thanks Rando!

I think you hit the nail on the head. To test your hypothesis I took an old shark PP from many years ago that I edited to cut clock gears (I vaguely remember reading a post online that walked me through the process of tightening up the tolerances). While it is not metric and it is very old I ran the PP just to see what it would do...It is cutting as I type this and the corners/points are square.

I hope you had a Merry Christmas and have a safe, healthy New Year.
Thanks again.

Andy

asever
Posts: 34
Joined: Fri Sep 03, 2010 12:17 pm

Re: Gcode Issue...I think

Post by asever »

Just double checking I am doing this right. Editing the Next Wave inch PP file in note pad I added "G64 P0.005" just below the "G90"...


+---------------------------------------------------
+ Commands output at the start of the file
+---------------------------------------------------

begin HEADER

"( [TP_FILENAME] )"
"( File created: [DATE] - [TIME])"
"( for Next Wave Automation from Vectric )"
"( Material Size)"
"( X= [XLENGTH], Y= [YLENGTH], Z= [ZLENGTH])"
"( Z Origin for Material = [Z_ORIGIN])"
"( XY Origin for Material = [XY_ORIGIN])"
"( XY Origin Position = X:[X_ORIGIN_POS], Y:[Y_ORIGIN_POS])"
"( Home Position)"
"( X = [XH] Y = [YH] Z = [ZH])"
"( Safe Z = [SAFEZ])"
"([FILE_NOTES])"
"(Toolpaths used in this file:)"
"([TOOLPATHS_OUTPUT])"
"(Tool used in this file: )"
"([TOOLS_USED])"
"([TOOLNAME])"
"(|---------------------------------------)"
"(| Toolpath:- '[TOOLPATH_NAME]' )"
"(|---------------------------------------)"
"G90"
"G64 P0.005" <--------added
"G20"
"[FC]"

Do I have this right?

For metric I will convert .005 inches to mm... .127 millimeters

Thanks again for the help.
Andy

Rando
Posts: 757
Joined: Tue Jan 06, 2015 3:24 pm
Location: Boise, ID
Contact:

Re: Gcode Issue...I think

Post by Rando »

Andy:

Yup, that's the place...be sure there aren't additional copies of the G90...G20 lines of code
down farther in the post file. They typically have a couple different reasons for outputting
the preamble: first toolpath, then at tool changes, things like that. Post are fun to read
through...if you're into that kinda thing.

Yes, you're right that in metric it should be G64 P0.127

Glad you're making it work :mrgreen:

Rando
=====================================================
ThomR.com Creative tools and photographic art
A proud member of the Pacific Northwest CNC Club (now on Facebook)

Post Reply