Tool radius compensation

Discussions around the CAM Add-On of QCAD.

Moderator: andrew

Post Reply
User avatar
andrew
Site Admin
Posts: 7413
Joined: Fri Mar 30, 2007 6:07 am

Tool radius compensation

Post by andrew » Fri Feb 05, 2021 11:48 am

From a QCAD/CAM user:
My machine does not offset / compensate the tool radius even though I'm choosing to cut outside or inside in QCAD/CAM.

User avatar
andrew
Site Admin
Posts: 7413
Joined: Fri Mar 30, 2007 6:07 am

Re: Tool radius compensation

Post by andrew » Fri Feb 05, 2021 11:50 am

You might be using a post processor which uses G41/G42 for tool radius compensation. This means that QCAD/CAM exports the contour data at its desired size and the machine controller computes the tool radius offset, not QCAD/CAM.

However, not every controller supports G41/G42. Please refer to your controller manual to find out if yours does. Otherwise, you would have to use a different post processor which exports computed offsets (e.g. "G-Code (Offset) [mm]"). In this case, QCAD/CAM computes the required offset.

Collen
Newbie Member
Posts: 3
Joined: Fri Feb 05, 2021 11:03 am

Re: Tool radius compensation

Post by Collen » Sat Feb 06, 2021 9:59 am

@ Andrew,

in my case, in the dialog box for tooling, practically I wrote 2mm as depth before generating , when I double checked after generating the depth is in the programme reads 4mm , before I even involve the controller.

User avatar
andrew
Site Admin
Posts: 7413
Joined: Fri Mar 30, 2007 6:07 am

Re: Tool radius compensation

Post by andrew » Sat Feb 06, 2021 11:12 am

Please attach your DXF file as this contains all the data we need to help you efficiently, thanks.

Collen
Newbie Member
Posts: 3
Joined: Fri Feb 05, 2021 11:03 am

Re: Tool radius compensation

Post by Collen » Tue Feb 09, 2021 7:40 am

HI, Andrew , Tool compensation

find attached dxf 1025
Attachments
1025PANEL.nc
(553 Bytes) Downloaded 19 times
PANEL1025.dxf
(140.67 KiB) Downloaded 22 times

User avatar
andrew
Site Admin
Posts: 7413
Joined: Fri Mar 30, 2007 6:07 am

Re: Tool radius compensation

Post by andrew » Tue Feb 09, 2021 10:13 am

Your Z levels are configured as follows:
Screenshot 2021-02-09 at 10.07.35.png
Screenshot 2021-02-09 at 10.07.35.png (26.04 KiB) Viewed 793 times
This means that:
- The safety level is Z=0. This is where the tool moves to in rapid mode.
- Your material starts at Z=-5
- The ultimate cutting depth is Z=-16
- You are cutting in two passes, first pass at Z=-10.5, second pass at Z=-16.

Looking at the G-Code file, I can see those Z values.

Note that usually the material starts at Z=0, your safety level would be at perhaps Z=2 and your cutting depth for example Z=-11 with the first pass at Z=-5.5 and second pass at Z=-11. However, your configuration can make sense depending on your use case.

I cannot see the depth "2" as you indicated nor the depth "4" you mentioned being generated. Can you please double-check?

I hope that helps.

Collen
Newbie Member
Posts: 3
Joined: Fri Feb 05, 2021 11:03 am

Re: Tool radius compensation

Post by Collen » Mon Feb 15, 2021 2:22 pm

@ Andrew,
I managed to sort out the issue of 5mm less on my work,
like you mentioned some machines are not compatible with G41/42 , like mine now am using Gcode offset mm, now the machine is producing excellent work its now 100% accurate thanks for the support .

Post Reply

Return to “QCAD/CAM”