Hole Spotting

I'm reasonably decent at CAD having used Fusion360 to design and 3D print for some time now.  However I'm a newbie (and I mean COMPLETE newbie) to CAM, gcode and post processors.  

I've built a 1500x1500mm downdraft plasma CNC table.  It's working rather well.  I've managed to get myself as far as the most basic of understanding manufacturing in Fusion.  Using the PP from the forum here I can get a flat pattern, generate a tool path and post it to an NC file and get parts cut with reasonable success.

I haven't figured out hole spotting though.  I know folks may say use something like Sheetcam and I'm sure it's a good solution but I'm trying to stay in Fusion (for now at least).

I tested QtPlasmaC's built in spotting function by writing a really simple gcode file to spot at the torch's current zeroed position and it works.  The built in spotting is quite nice actually.  Leaves a perfect little dimple (I'm testing with 1/8" aluminum sheet).  500ms pulse@20A

Before I try to reverse engineer the Fusion360 post processor to figure this out I'm wondering if there's any cool tricks in Fusion to get the PP to write the M3 $2 S1 command at a specific point.  

Or as a reasonable work around get it to write something out that's easy to search and replace with M3 $2 S1.   If that makes sense.

I did see something about adding in a drilling operation but when I tried it I discovered the free version of Fusion won't allow that.

Also not sure why the G91/G1microscopic move is necessary.  Pretty sure the tolerance settings will result in it being ignored but without it I get an error loading the file that it'll move outside my machine boundary.  I don't think that's the case but QtPlasmaC still throws the error.

Anyway I hope this isn't a bunch of utterly annoying newbie questions.    I sincerely appreciate any help with this part of the learning curve.

Cheers,

-Dave
 

Can't help in fusion but in Sheetcam you can create layers and you can define the minimum diameter of holes you can cut (say 12mm) so you move all of the small holes onto a new layer. When you generate the code for that layer  it will create the spots at the hole centre.
The torch won't fire if there is no movement in the following segment so move to relative coordinates to move a tiny amount to keep LinuxCNC happy and make the torch fire.

So now see if you can translate that to fusion.

dlv wrote:

I'm trying to stay in Fusion (for now at least).
 

In my opinion using Fusion for plasma (or laser) is like bought truck for drive to church - more troubles than benefits.
My favorite option is Librecad plus dxf2gcode - GPL and cost free.
Try this, even if you will not like them, this is simple and you will easy learn something.

Actually one way to do this would be to write a gcode filter for linuxCNC  that looked for hole below a certain diameter, removed the hole processing and replace it with a spot at the hole centre. Monokrom plasma has a filter that modifies hole processing so perhaps it can help you.

Another really out there possible solution that does not need post processing (but requires master branch) could  be to write a component or modify plasmac.comp and monitor the pin motion.interp.iscircle. When it goes true and motion.interp.arc-radius < minimum hole radius, disable the torch, use external offsets to move a distance of motion.interp.arc-radius along motion.interp.normal-heading (which will be your hole centre), fire the torch to spot, then unwind the offsets to return to where the torch was, let motion take over again then enable the torch when iscircle goes false.(the end of the hole)

Thanks Rod.  Fusion has cut profiles.  The approach would be similar to the layers you mention I think.  Select the holes to be spotted in one cut profile and the rest of the part sans the small holes in another.  Perhaps a bit more "one click" in Sheetcam but it's really no trouble in Fusion.  Then from the two profiles I post two different NC files so I can change my torch amps between spotting and cutting (I have to do that manually, no fancy Hypertherm for me!).

I will look into writing a gcode filter take small holes and replace with the spotting commands I have in my test code.  That's the approach I've been thinking of anyway.  Was wondering if anyone had already done that.  If there are examples out there of gcode filters anyone can point me at I'd appreciate it.  I've got decent C and Python skills.

Tommy I looked at the feature I think you're referring to and from what I read QtPlasmaC will take a gcode command to only run the pierce operations it finds in the file and no cut ops.  I guess I'd use the cut profile approach above with just the holes in it and set the lead in to put the torch in the hole center for the pierce.  Like 2mm holes with a 1mm 90deg lead in.  Then use this: So yeah that would be ok if I wanted to actually pierce the hole centers.  I like the "center punch" dimples I'm getting with the M3 command test above but this certainly would be a solution to try and I will.  Might work better on thicker steel.  So far I'm just testing on aluminum sheet.

tuxcnc I'll check out dxf2gcode.  I can export a DXF and post process that.  You're not wrong, Fusion is a beast.  But I'm really quite comfortable on the design side and for the most part I like working with it.  That said since I'm learning the CAM side I am definitely open to trying some alternatives especially if they're open source.

Thanks guys!

dlv wrote:

tuxcnc I'll check out dxf2gcode.  I can export a DXF and post process that.  You're not wrong, Fusion is a beast.  But I'm really quite comfortable on the design side and for the most part I like working with it.  That said since I'm learning the CAM side I am definitely open to trying some alternatives especially if they're open source.

 

I'm not against Fusion if the user paid for commercial version.
I'm against the "free" versions (student, hobby, etc.), because someday thats may become won't start without any warning.
However Fusion is large program with thousands functions, so the good question is it worth learn this for simply projects...
I suggested Librecad plus dxf2gcode not because this is Fusion replacement (is not), but because it is very simple and enought for simple projects.
In Librecad you easy can place small circle at the center of big circle, and in dxf2gcode yo can learn the edition of postprocesor  in one hour, because it is plain text human readable.
For example this is fragment of my laser postprocessor:My laser has no Z axis, so no lines for Z moves, but the feed of Z move is simply translated to laser power (F -> S).
I don't know how is in Fusion (I'm not curious about it), but I think this is more complex. In some CAM you can nothing without programming knowlege...

 

FWIW the "pierce only" feature is the answer for me in my workflow.  This along with selecting the holes to be center pierced into a separate Fusion 2D cut profile with the path parameters set to center offset, 90 deg lead in, lead in = 1/2 the circle diameter worked perfectly.  Since size doesn't matter (pun intended) I just used 6mm circles with 3mm lead in.  No gcode editing or other steps needed.

Thank you Tommy for prompting me to RTFM.   I was a dolt and didn't even realize that the "Normal Cut" button in the GUI toggles "Pierce Only"!  I was stuck on trying to use the M3 $2 S1 code but this works just fine.

I did also create a material.cfg entry for "Hole Spotting" and put my center piercing settings in there; 0.120" pierce height, 20A (as low as my machine will go) and 0.1s Pierce Delay (as short as it will go).  I'll add more as needed for thicker materials.

Cheers!
 

I think from memory, in sheetcam, you do a drill operation and that inserts the spotting code. (assuming its in the post processor) Perhaps you can do the same in f360.