Path in Fusion360 different from actual path
20 May 2021 14:55 #209657
by mf290997
Path in Fusion360 different from actual path was created by mf290997
Hi,
I have the issue, that on moves between cuts, the CNC starts moving in X/Y before Z is fully lifted out of the hole. That very often kills the cutter. In Fusion360 those linking moves are shown as perfectly rectangular moves. The Previewer in LinuxCNC shows the linking moves with an arc at the top, where Fusion360 shows a sharp corner.
Does anybody know why this is, and how to prevent this issue?
Thanks,
Max
I have the issue, that on moves between cuts, the CNC starts moving in X/Y before Z is fully lifted out of the hole. That very often kills the cutter. In Fusion360 those linking moves are shown as perfectly rectangular moves. The Previewer in LinuxCNC shows the linking moves with an arc at the top, where Fusion360 shows a sharp corner.
Does anybody know why this is, and how to prevent this issue?
Thanks,
Max
Please Log in or Create an account to join the conversation.
20 May 2021 15:34 #209660
by AgentWD40
Replied by AgentWD40 on topic Path in Fusion360 different from actual path
Please Log in or Create an account to join the conversation.
- tommylight
-
- Away
- Moderator
-
Less
More
- Posts: 18563
- Thank you received: 6220
20 May 2021 15:40 #209661
by tommylight
That was discussed here on the forum lately but i can not find the topic, not sure what happened later but you might want to try to update LinuxCNC.
Replied by tommylight on topic Path in Fusion360 different from actual path
That was discussed here on the forum lately but i can not find the topic, not sure what happened later but you might want to try to update LinuxCNC.
Please Log in or Create an account to join the conversation.
20 May 2021 16:32 #209664
by Sandro
Replied by Sandro on topic Path in Fusion360 different from actual path
I had something similar once while engraving. Sharp corners were rounded off because by default the G64 command was active. That also occurred during lifting of the tool.
Please Log in or Create an account to join the conversation.
20 May 2021 16:46 #209666
by mf290997
Replied by mf290997 on topic Path in Fusion360 different from actual path
It looks like G64 could be the issue. How can I disable that? Nowhere in my GCode I can find a G64. Is it somewhere in the machine configurations?
Please Log in or Create an account to join the conversation.
20 May 2021 17:02 #209668
by AgentWD40
Replied by AgentWD40 on topic Path in Fusion360 different from actual path
It's enabled by default. Have a look at the docs I linked above, it shows how to disable it are maybe better to adjust the tolerance to a small number. It's just a gcode command, you can add it to your pp.
Please Log in or Create an account to join the conversation.
20 May 2021 18:04 #209674
by Michael
Replied by Michael on topic Path in Fusion360 different from actual path
Either add G61 to the top of each g code file or manually enter it in the mdi prior to starting a program. That will be exact path following.
I prefer to leave a bit of blending and usually do a G64 P.003 or G64 P.005 to each file to make sure it's always used with the file.
The lower acceleration your machine is capable of the more it will cut corners in G64 mode with no tolerance. Putting a bit of tolerance P will keep it from cutting corners and also not come to a complete stop like a G61 will on occasion
I prefer to leave a bit of blending and usually do a G64 P.003 or G64 P.005 to each file to make sure it's always used with the file.
The lower acceleration your machine is capable of the more it will cut corners in G64 mode with no tolerance. Putting a bit of tolerance P will keep it from cutting corners and also not come to a complete stop like a G61 will on occasion
Please Log in or Create an account to join the conversation.
24 May 2021 00:41 - 24 May 2021 00:42 #209962
by BigJohnT
It's not something you disable, it's the default if you don't specify something else in your preamble.
Example of good preamble
gnipsel.com/linuxcnc/g-code/gen01.html
JT
Replied by BigJohnT on topic Path in Fusion360 different from actual path
It looks like G64 could be the issue. How can I disable that? Nowhere in my GCode I can find a G64. Is it somewhere in the machine configurations?
It's not something you disable, it's the default if you don't specify something else in your preamble.
Example of good preamble
gnipsel.com/linuxcnc/g-code/gen01.html
JT
Last edit: 24 May 2021 00:42 by BigJohnT.
Please Log in or Create an account to join the conversation.
Time to create page: 0.091 seconds