Pausing at Nodes

More
28 Jan 2021 02:23 #196878 by CBEAR
Pausing at Nodes was created by CBEAR
I've been experiencing a problem the last few times that I've been cutting. I'm cutting out some large commerical signs with very simple/large letters. The last few jobs that I've done I've noticed that my machine slows down significantly at each node. Each letter has 4-8 nodes total depending on the letter. Even on arcs that are as smooth as can be (example: the letter "O") it will slow way down at each node. At first, I thought that it may be my cut rules slowing it down, so I tried it again without any cut rules, and it cut exactly the same. I have my following tolerance set at the standard .010" and it hasn't done this before. It just started a few weeks ago.

Please Log in or Create an account to join the conversation.

More
28 Jan 2021 03:09 #196884 by phillc54
Replied by phillc54 on topic Pausing at Nodes
If you use the standard SheetCam postprocessor then it may be worth a try changing the following in the GCode file:

From:
G64 P0.01 Q0.001 (tracking tolerances: 0.01")

To:
G64 P0.01 (tracking tolerances: 0.01")

Please Log in or Create an account to join the conversation.

More
28 Jan 2021 03:11 #196885 by CBEAR
Replied by CBEAR on topic Pausing at Nodes
I'll give it a shot. Is there a way that I can take it out of the post so that I don't have to remove it from every gcode file? If not, that's fine too.

Please Log in or Create an account to join the conversation.

More
28 Jan 2021 03:14 #196886 by phillc54
Replied by phillc54 on topic Pausing at Nodes
Sure, it is in the current postprocessor at line 72, it looks like:
    if scale == metric then
        post.Text (' G64 P0.254 Q0.025 (tracking tolerances: 0.254mm)\n') 
    else
        post.Text (' G64 P0.01 Q0.001 (tracking tolerances: 0.01")\n') 
    end
just change it so it looks the same.

Please Log in or Create an account to join the conversation.

More
06 Feb 2021 18:53 #197861 by CBEAR
Replied by CBEAR on topic Pausing at Nodes
Is this the spot that I need to change? Still having a lot of issues with it slowing down at a really small area that the table shouldn't have any issues keeping up the velocity in.

Please Log in or Create an account to join the conversation.

More
06 Feb 2021 18:58 #197862 by CBEAR
Replied by CBEAR on topic Pausing at Nodes

phillc54 wrote: Sure, it is in the current postprocessor at line 72, it looks like:

    if scale == metric then
        post.Text (' G64 P0.254 Q0.025 (tracking tolerances: 0.254mm)\n') 
    else
        post.Text (' G64 P0.01 Q0.001 (tracking tolerances: 0.01")\n') 
    end
just change it so it looks the same.


I have revision F if that makes a difference

Please Log in or Create an account to join the conversation.

More
06 Feb 2021 21:34 #197873 by CBEAR
Replied by CBEAR on topic Pausing at Nodes
It seems to have been a sheetcam issue with import tolerances being too small!
The following user(s) said Thank You: phillc54, snowgoer540

Please Log in or Create an account to join the conversation.

More
06 Feb 2021 21:43 #197874 by snowgoer540
Replied by snowgoer540 on topic Pausing at Nodes

CBEAR wrote: It seems to have been a sheetcam issue with import tolerances being too small!


Happy we finally got this figured out!!

To anyone following along, we changed this import setting in sheetcam:
Max detail reduction error
from the default of 0.0004" to 0.010"

Per sheetcam manual:

Max detail reduction error
Some drawings consist of a large number of very small line segments (especially polyline curves converted to DXF). This can slow down processing and produce very large g-code files. It can also slow down machining. SheetCam tries to reduce the number of lines when it loads the drawing. Removing lines introduces small errors and this value is the maximum allowable error. For Plasma cutting you can afford to have quite a large error (say .020"). The setup wizard adjusts this value to suit.

The following user(s) said Thank You: phillc54

Please Log in or Create an account to join the conversation.

Moderators: phillc54
Time to create page: 0.096 seconds
Powered by Kunena Forum