Reducing the amount of start points.

[Creative25]

I am cutting small letters out of a 10 mm plate.
My problem is that the nozzle wears badly during pearcing.
So I would like to reduce the amount of starts.
First cut the holes in the closed letters o e R etc. Then cut the outside of all the letters without the torch turning off.
Is there a function on Sheetcam that can do this or do I need to modify the drawings?

[djreiswig]

In operation set the maximum chain length to something large and it should chain cut. Not sure if it will cut all inside cuts first or not.

[sheetcamCS2]

In the Jet Operation window, see 'Max chain length'. Chaining keeps the torch on and down between shape cuts. See Help on the topic also.
Also combine it's use with a small negative 'overcut' (aka undercut), suitable lead in and lead out, and cut path 'shortest path' for auto toolpath layout which should approximate your intentions. You can always edit the start points to further facilitate chaining of shape cuts.
In this example, the toolpath was auto layout, that is no edited start points.

[adbuch]

In operation set the maximum chain length to something large and it should chain cut. Not sure if it will cut all inside cuts first or not.

[Creative25]

Thanks
So the function I was looking for is the chain function that seems pretty simple.
What does the function undercut -0.5 do?
I’m thinking of moving the holes in the letters to another layer so I can have the correct lead ins.
Does Sheetcam have a function to start leading for holes in the center?

[sheetcamCS2]

What does the function undercut -0.5 do?

Because I used perpendicular leadin and leadout, it keeps them from overlapping, so the arc is well fed through the whole toolpath. I chose perpendicular to give sheetcam a good chance at auto gen the toolpath in this circumstance, however other styles may work fine also, I didn't try them.

Does Sheetcam have a function to start leading for holes in the center?

yes it does, on that same Operation window (at bottom) and also on Tool definition window, the Operation values will override the Tool def values.

Here is some good new user info to read and videos to watch- https://forum.sheetcam.com/t/where-to-l ... cam/8102/2
and here- https://forum.sheetcam.com/t/toolset-pr ... ricks/8281

[djreiswig]

Does Sheetcam have a function to start leading for holes in the center?

yes it does, on that same Operation window (at bottom) and also on Tool definition window, the Operation values will override the Tool def values.

I assumed the start in center of holes only worked on circles, and not the irregular internal shapes in his drawing.

[sheetcamCS2]

I assumed the start in center of holes only worked on circles, and not the irregular internal shapes in his drawing

Your assumption is correct, only for holes which are true circles. I had equated "holes" to "circles" in my former reply, good point that you clarified that.

TMI warning... I only mention this because it can be a serious 'head scratcher' when sheetcam doesn't recognize a circle.
While we're on the topic of circles as holes, it's worth noting that sheetcam has more than one algorithm to recognize holes as circles for center starting vs. drilling. I was advised by Les some time ago that dxf files (polylines) can present a more accurate arc in the drawing for such recognition than do svg files w bezier curves or b-splines. This can vary by CAD, CAD settings, size of circle, and sheetcam settings (menu Options-'Application options'-'Drawing import'). I have used dxf files ever since with near 100% success of circle recognition, the exceptions being when polyline arc tolerance settings are seemingly out of sync between CAD and sheetcam, usually due to a settings reset or some other inadvertent settings change. In sheetcam, see 'max detail reduction error' in the settings window cited above.

An example of the same when CAD exports dxf is best described here as 'curve tolerance' - https://docs.lightburnsoftware.com/1.7/ ... t-settings, with attribution to Lightburn sw.

[adbuch]

I assumed the start in center of holes only worked on circles, and not the irregular internal shapes in his drawing

Your assumption is correct, only for holes which are true circles. I had equated "holes" to "circles" in my former reply, good point that you clarified that.

TMI warning... I only mention this because it can be a serious 'head scratcher' when sheetcam doesn't recognize a circle.
While we're on the topic of circles as holes, it's worth noting that sheetcam has more than one algorithm to recognize holes as circles for center starting vs. drilling. I was advised by Les some time ago that dxf files (polylines) can present a more accurate arc in the drawing for such recognition than do svg files w bezier curves or b-splines. This can vary by CAD, CAD settings, size of circle, and sheetcam settings (menu Options-'Application options'-'Drawing import'). I have used dxf files ever since with near 100% success of circle recognition, the exceptions being when polyline arc tolerance settings are seemingly out of sync between CAD and sheetcam, usually due to a settings reset or some other inadvertent settings change. In sheetcam, see 'max detail reduction error' in the settings window cited above.

An example of the same when CAD exports dxf is best described here as 'curve tolerance' - https://docs.lightburnsoftware.com/1.7/ ... t-settings, with attribution to Lightburn sw.
Screenshot 2025-05-06 083230.png

[Creative25]

Thanks that clarifies a lot.
So it would be better to add the lead ins for letters as straight lines and change the length till it is more or less in the middle.

Now a have another question.
I am planning to mark the start points of the inside cuts first. Plasmac has an option pierce only.
I was thinking of using this function with a very low pierce delay say 0.05 seconds. Then drill holes. So in the end I can do the cutting with edge starts only.

Will this work?
Or will the mark be hardened to such an extent that drilling will be difficult?

[djreiswig]

What plasma cutter are you using? On thicker material I've had good luck using a ramp pierce. Set the plunge rate the same as the feed rate. This tends to shoot the junk behind the torch rather than up into it. I've cut a fair amount of 1/2" this way.

[adbuch]

Thanks that clarifies a lot.
So it would be better to add the lead ins for letters as straight lines and change the length till it is more or less in the middle.

Now a have another question.
I am planning to mark the start points of the inside cuts first. Plasmac has an option pierce only.
I was thinking of using this function with a very low pierce delay say 0.05 seconds. Then drill holes. So in the end I can do the cutting with edge starts only.

Will this work?
Or will the mark be hardened to such an extent that drilling will be difficult?

Yes - I think pre-drilling your pierce points will work fine, and will most likely extend your consumable life vs. doing actual pierces in that thick material.

David

[Creative25]

What plasma cutter are you using? On thicker material I've had good luck using a ramp pierce. Set the plunge rate the same as the feed rate. This tends to shoot the junk behind the torch rather than up into it. I've cut a fair amount of 1/2" this way.

I have a power max 45 do to insufficient electricity I can only cut at 35 amps else the voltage on the supply line drops too much and the plasma cutter cuts off and gives a warning. With 35 amps on a 10mm sheet it takes 2 seconds to Pearce through.

[adbuch]

What plasma cutter are you using? On thicker material I've had good luck using a ramp pierce. Set the plunge rate the same as the feed rate. This tends to shoot the junk behind the torch rather than up into it. I've cut a fair amount of 1/2" this way.

I have a power max 45 do to insufficient electricity I can only cut at 35 amps else the voltage on the supply line drops too much and the plasma cutter cuts off and gives a warning. With 35 amps on a 10mm sheet it takes 2 seconds to Pearce through.