Custom version of Fusion 360 post processor to enable "pierce only in the center" for holes

I have made this post processor if you are interested in having Fusion just pierce the center of (some) holes so that they can be driller/reamed manually.

This version is distributed in the hope that it will be useful, but WITHOUT ANY WARRANTY; without even the implied warranty of MERCHANTABILITY or FITNESS FOR A PARTICULAR PURPOSE

It installs like the regular one from Langmuir but it’s marked 1.7 just to differentiate it.

In order to use it, create a cut operation and name it “pierce-only”. You can have other operations (with different names) for regular cuts. Typically you want to pierce holes first and then cut other shapes, but there is nothing in this modified post processor to require or enforce that.
image

It is important that the “pierce-only” cut operation does not use any lead-in, lead-out and that Pierce Clearance is set to 0 and consists of circular holes only. The post processor tries to detect failure to do so but it cannot be not fool proof.
image

When ready to post-process, make sure to enable this designated function.

The resulting G-code will only pierce in the center of the hole (make sure your pierce delay is adequate, but so any other parameter of the cutter):
image

I am still not sure in what language this post-processor is written in.

The code is now still under review in a branch on my github; if you know how to do, please have a look. In the future I might make a “release”.

4 Likes

Hi @manoweb

Thank you for this! I’m working with a friend who has a Langmuir to help him learn Fusion 360. I tested out the PP today on my Mac, and had no trouble posting G-code. But when we were trying the same on his PC, we kept getting an error. Paraphrased, it was “no linear cuts allowed, turn off lead-in, lead-out and set pierce clearance to 0. Post failed.” Digging deeper, it directed us to line 478 of the PP.

The resulting .nc.failed file looked exactly the same as my successful one, except that it had a line at the end declaring it failed. Otherwise, I couldn’t spot a single difference (except his was inches G20 and mine mm G21).

(v1.6-af)
G90 G94
G17
G21
H0

(pierce-only)
(Piercing center of hole only)
G0 X-39.964 Y21.9
M3
G4 P0.5
M5
G0 Z25.4

M30
(PS0)

But we’d followed your instructions to a T: toolpath named “pierce-only”, lead-in & out off, pierce clearance 0. I even fiddled with the passes tab, switching between left and center offset compensation. And the selected geometry was a series of circular holes, specifically the top edges selected. (The above G-code is truncated to just one such hole). In NC Program we checked “Center pierce only detect,” turned off THC & IHS, had no spaces in the file name…

Any ideas? We changed the extension on the failed file to just .nc and he’s going to run a test with it, but it’d be great if we could get it working as intended.

Thanks!

Milan

Interesting. Would you be so kind to attach the .f3d of your Fusion design for me to try?

In practice, that error message means Fusion is trying to perform a linear cut on the layer that is supposed to be center pierces only.

Is this Post Processor available to try? THank you.

Sure I’ll repackage and send it to you tomorrow. If it works for a few people I’ll make it easily downloadable

2 Likes

Add me to the list please.

I need to drill some precision holes in some 3/4 plate, and this will save having to draw out the dimensions on the cut pieces if I can locate on certain points (PITA on curves).

I went to the Github site and downloaded that cps file, but my Fusion360 said invalid file and will not add to the post processors.

THank you in advance.
Greg

Yes I am actually quite happy people want to try it out. I tested it more today as I haven’t used the plasma cutter in a few weeks due to unrelated reasons. I will send it out to interested people as soon as I’m done with a couple of other cuts and provide guidance on how to install it

3 Likes

I’d like to try it out also. Would be a good option when accuracy is needed and tolerance’s are tight

Thanks…I did a quick design and created the g-code without issue. I haven’t tested it out but seemed to work for me. I posted the 5 hole design.

(v1.6-af)
(Machine)
( vendor: Autodesk)
( model: Hypertherm 45)
( description: Generic Cutting Machine)
G90 G94
G17
G20
H0
(pierce-only)
(Piercing center of hole only)
G0 X4. Y4.
M3
G4 P0.6
M5
G0 Z0.

(Piercing center of hole only)
G0 X2.5 Y2.5
M3
G4 P0.6
M5
G0 Z0.

(Piercing center of hole only)
G0 X1. Y4.
M3
G4 P0.6
M5
G0 Z0.

(Piercing center of hole only)
G0 X1. Y1.
M3
G4 P0.6
M5
G0 Z0.

(Piercing center of hole only)
G0 X4. Y1.
M3
G4 P0.6
M5
G0 Z0.

(2D Profile3)
G0 X5.05 Y-0.05
M3
G4 P0.6
G3 X5. Y0. I-0.05 J0. F100.
G1 X0. F150.
G1 Y5.
G1 X5.
G1 Y0.
M5
G0 Z0.

M30
(PS150)

1 Like

Hey guys sorry, I’m having trouble with the Internet connection to my computer at home. I’ll fix it tomorrow, now I’m posting this with the phone. I’ll take care of all the requests I received!

3 Likes

It worked great! Marked all the holes exactly as you said it would. Thanks again


2 Likes

@DonP - So is that post to you or is that the post you downloaded off of GitHub?

I tried the one off github, and no change. Trying to figure out what I am doing wrong.

I got mine from Alessio. Send him a message and I believe he is giving them out but wanted to wait to make sure it worked as expected before posting it and giving instructions.

1 Like

I noticed that there is no IHS probing sequence and the retract is to Z zero. Are you setting the torch height manually?

Yes, I set manually but sure you can use IHS if you wanted.

1 Like

Hello, sorry my computer literally broke. I am now back online.

Hey guys to make it easier I’m attaching it here for the time being. Once I got some more feedback, I will choose a more proper location.

FireControl-v1.7.cps.zip (5.1 KB)

3 Likes

By the way I improved a couple of things where due to Fusion’s approach the PostProcessor would try to send multiple center-pierce for the same hole and add the possibility to have several cut operations with a name that starts with pierce-only. Here is the newest version. Sorry, version control on a forum post is horrible but that’s what I have
CrossfireFusion360PostProcessor-pierce-only.zip (5.9 KB)

The same code is available at:

3 Likes