QCAD.org Forum

Hello,

First of all, please excuse me if I don't use the right vocabulary, I have the french trial version 3.30.1 of QCAD/CAM (I bought it in 2017 but thought that I could use an update)
For the context I have a plasma table to cut mostly 2mm steel. I sometimes have small or shallow holes that are not easy to start without damaging the part with the peircing...

I checked several "Plasma" post-processors and I don't understand why the only tools you can add are "Mills" and "Drills" where "Laser" post-processors have the "laser" tool. I could create a post-processor later if needed...
Then I tried to set the entry to eighth of circle but "mill" shoud start from center of the arc and cannot start on the arc (must be some plunging reason for milling) So I tried some "Laser" post-procesosrs with the "laser" tool (with 1.5mm in diameter) and set the entry to eighth of circle with a radius of 5mm. It does look like it works at first but the 5mm radius is applied to the "normal" path and the offset path starts directly from that point. In some configurations, depending on the curvature of the path, it results in getting the peircing point between the normal path and the offset: it will be seen in the final part... I can understand that the radius be applied to the normal path and not to the offset path, but the tool still has a diameter (thus a radius) which is not taken into account... And I think the laser tool was thought with a 0mm diameter and more for engraving or cutting paper thant cutting steel

Both (mill and laser) path look like what would happen if milling with a 45° mill an plunging progressively...

What would be correct for plasma (and laser) is that both arcs ("normal" and "offset" have the same center). I hand made this: The circle would represent the minimum peirced hole (could even be bigger to be realistic)

A variable length or angle would also be preferable to only half/quarter and eighth...

I could not find the definitions of the tools and how the offset is made so I cannot modify this myself

Or did I miss something ?

If you need more info on the plasma cutting process, I will try to provide as much as I can

Hi,

The only difference with a mill or a drill is that a laser is not a rotational cutting tool.
The naming and the purpose of the tool doesn't matter at all.
Simply set a certain small spot diameter for proper offsetting.

About the offset Lead-in and Lead-out.
Already reported in detail here:
https://www.qcad.org/rsforum/viewtopic. ... 206#p44206
I called them "donkey ears".
The entry and exit paths can indeed ruin your piece.
It is not limited to eighth of circle: https://www.qcad.org/rsforum/viewtopic. ... 107#p45107

The Bug report is here:
https://qcad.org/bugtracker/index.php?d ... sk_id=2558
Remark the "Won't fix" but I filed a request to re-open the task.

Regards,
CVH

cool.occd: Thanks for your detailed report.

I've opened a bug report at:
https://qcad.org/bugtracker/index.php?d ... sk_id=2584

I can confirm that this should be fixed for the next release. The start point of the offset toolpath should only coincide with the start point of the original toolpath if G41/G42 is used.

Thank you very much.

You may disregard or clear the request to re-open the task FS#2558

Kind regards,
CVH

Hello, thanks for your replies.

CVH wrote: ↑

Tue Jul 09, 2024 9:05 pm

The only difference with a mill or a drill is that a laser is not a rotational cutting tool.
The naming and the purpose of the tool doesn't matter at all.
Simply set a certain small spot diameter for proper offsetting.

I have set the diameter to the "kerf" width, so no problem with the offset in general.
I understand that laser and plasma don't rotate and mill and drill do rotate, but what makes that mill can't make a "not from center" lead in ?
So "my" plasma tool is simply a working laser tool I still don't understand why plasma post-processors use a mill instead of the laser...
I don't know for the laser, but a plasma tool could have another parameter for controlling the torch height control (THC): the arc voltage (well my cnc doesn't need it to be defined in the GCODE but some other cnc might...)

CVH wrote: ↑

Tue Jul 09, 2024 9:05 pm

About the offset Lead-in and Lead-out.
Already reported in detail here:
https://www.qcad.org/rsforum/viewtopic. ... 206#p44206
I called them "donkey ears".
The entry and exit paths can indeed ruin your piece.
It is not limited to eighth of circle: https://www.qcad.org/rsforum/viewtopic. ... 107#p45107

The Bug report is here:
https://qcad.org/bugtracker/index.php?d ... sk_id=2558
Remark the "Won't fix" but I filed a request to re-open the task.

I couldn't find those other topics because I had not the "lead in" term right... sorry...
Of course other partial circle should have the same problem if they use the same algorithm, I may even have tried it but forgot to mention it

andrew wrote: ↑

Wed Jul 10, 2024 7:57 am

I can confirm that this should be fixed for the next release. The start point of the offset toolpath should only coincide with the start point of the original toolpath if G41/G42 is used.

Thanks!!
I didn't even try G41/G42 because I simply don't know if my cnc can handle it...


It maybe another topic, but one other thing that kind of bothers me concerning the offset that can be seen in your "lead_in_offset.png" is the fact that the "normal" path is made of the original polyline (let's say) segments and thus don't really take into account the tool radius. Would it be possible to regenerate the "normal" path by offsetting the "offset" path ? or create another "result" path ?

Have a nice day

cool.occd wrote: ↑

Fri Jul 12, 2024 8:59 am

It maybe another topic, but one other thing that kind of bothers me concerning the offset that can be seen in your "lead_in_offset.png" is the fact that the "normal" path is made of the original polyline (let's say) segments and thus don't really take into account the tool radius. Would it be possible to regenerate the "normal" path by offsetting the "offset" path ? or create another "result" path ?

The "normal" path is part of the internal structure of QCAD/CAM that represents a toolpath. Each toolpath is generated into a block with a copy of the original entities, the normal toolpath (cutting edge) and the offset toolpath among other things. When exporting with G41/G42, the normal toolpath geometry is exported, when exporting without G41/G42, the offset toolpath geometry is exported. If you want to hide the normal toolpath, you can simply hide the layer "normal" of your post processor in the layer list.

andrew wrote: ↑

Fri Jul 12, 2024 9:06 am

The "normal" path is part of the internal structure of QCAD/CAM that represents a toolpath. Each toolpath is generated into a block with a copy of the original entities, the normal toolpath (cutting edge) and the offset toolpath among other things. When exporting with G41/G42, the normal toolpath geometry is exported, when exporting without G41/G42, the offset toolpath geometry is exported. If you want to hide the normal toolpath, you can simply hide the layer "normal" of your post processor in the layer list.

Hi,

It's not about hiding the "normal" path...

What I meant was that you will not have the part cut AS the normal path because of the tool radius, i.e. internal acute cuts will have a radius corresponding to the tool thus the part will be less "pointy" (well... less negatively pointy as it will apply only for concave angles)
And so it would be interresting to be able to visualise the "real" cut part, instead of the one you are trying to make...

cool.occd wrote: ↑

Fri Jul 12, 2024 4:21 pm

And so it would be interresting to be able to visualise the "real" cut part, instead of the one you are trying to make...

That would be a game-changer.
Especially with pocketing in relation with engravings.
For the moment I use left and right offsets of the cutter path and fill that.
That may reveal 'uncut' areas or optimizing capabilities.
Some coin size designs can take hours to engrave ... Then a 10, 15 or even 25% gain in production time does count.
An imperfect end result is inexcusable and very expensive.

BTW: G41/42 and a curving Lead-in is mostly not supported.
There is no linear compensation path to an arc that is itself an arc.

Regards,
CVH