Shapeoko XXL , Carbide motion do not stop the spindle for me to install the tool


(Alain St-Laurent) #1

When I start a job, carbide motion prompt a message to install the tool, but do not stop the speedle for me to do so.
I’m using Fusion 360 with the Carbide 3D post-processor. For now I Install the tool before I sart the job.
Not a big deal for me at this time.


(Julien Heyman) #2

Yep this message is slightly confusing, it is more an opportunity to double check that everything is OK before proceeding to run the job. The (stock) shapeoko has no control on your router/spindle anyway, unless you wired a VFD to the controller board.
In any case you need to have zeroed before clicking this popup, so installing the endmill and zeroing beforehand is mandatory.


(Alain St-Laurent) #3

Thanks for the quick answer. I did installed a relay


(William Adams) #4

With a relay, the spindle should stop — if you have the correct G-Codes in the file and everything configured correctly.

We still recommend discrete files for each tool:


(Alain St-Laurent) #5

the code is issue by Fusion 360 build-in post processor, I did not edit or created any code, should be interested to find out if i’m the only one with that problem. I will read the info about tool changes.
I do create a cn file per tool.


(Alain St-Laurent) #6

I think I was wrong about Fusion 360 Carbide 3D post processing issuing the start and stop when Carbide motion prompt that meesage., I think?? It is Carbide Motion that control that …no?

I did read the document , thanks
Two things come up,

  • I just realsed the text said " we are starting a new job, we need to clear any existing offsets

Click the ‘Clear All Offsets’ button." I never did that step. Not sure what will be the drawback of not doing that step, could be just that if I shut down I can not go back to my last job origin??

  • After a job stop my XXL go to the back right corner not the center back?

(William Adams) #7

Carbide Motion will move the machine around and start/stop the spindle based on its interpretation of G-Codes in the file — I believe you need a special or modified post-processor for Autodesk Fusion 360.

Back right corner is I think the difference between M2 and M30.


(mikep) #8

Check the box for “minimize tool changes.” You won’t get this any more.

Yes, fusion360 is issuing the start. CM with nomad issues a stop, then move the carriage, then turns on the spindle again. SO3 doesn’t have all the parts to do that properly. Without something to control the router, obviously, it can’t turn off the power to the router.


(Alain St-Laurent) #9

Thanks , I will do that, on my SO3 I have installed a relay using the controller pwm output so just to say.


(Alain St-Laurent) #10

I am using the Carbide 3D post processor give by Fusion 360 for carbide motion controller, I pretty sure I have the latest, not that it matter that the spindle go back right corner or back center after a job stop, but i’m sure it’s not a flaw in the code, someone decided that it will,go to the back right corner when it creates that code.


(Neil Ferreri) #11

So the spindle turns on, then Carbide Motion asks you to insert a tool?
Can you share your gcode?


(Alain St-Laurent) #12

I am new to this , so as soon as I get back to my computer , I will figure how to attach a file , or wurst case I copy paste the nc file I guest.


(William Adams) #13

Make a very simple file and post the G-Code here and let us know what post-processor was being used and describe step-by-step the machine behavior.

We’ll work with you to compare it to: https://wiki.shapeoko.com/index.php/G-Code and puzzle out why the machine is doing what.


(mikep) #14

Ok, so here’s the deal. The CM preprocesses commands, and interprets T g-codes. That’s how it does tool changes on nomad. It’s broken on shapeoko. If you do a tool change using any post with SO3, CM will “sort of” interpret it. If the spindle is off, it will turn it on. It interprets the T command and the spindle on/speed command out of order. It’s broken. It’s been reported. More than once.

It doesn’t work properly with CM. CM does things worse than just ignoring the toolchange, it does totally wrong things.

You can’t use T commands on SO3 with CM.

GRBL doesn’t do T commands, which is why you’re getting the advice to use separate files.


(Alain St-Laurent) #15

You ask for one of my file, i send it to you by email.

the Fusion 360 post processor I use is
Carbide 3D GRBL ver 42201 21nov2018

the step by step is

I load one cn file one operation and one tool only.

So load the file

spindle home itself

I clear all offset

i position the spindle with the cutter at the x,y,z 0,0,0, for the job

i go to the run page and start run

the spindle move Z up and keep x,y to 0 and start the spindle

at the same time display a message “tool change required” “Insert tool #24 and click ok to continue” (it give me #24 because I put in FS360 the tool manager in the post processor tab a tool number it my way to store my cutters

I physicaly do nothing and I it continue and the job start.


(Alain St-Laurent) #16

Thanks , now i’m confused … in a fun way, i did not learn g-code yet, but I mention before that I create one file one tool/cutter, so sometime the one operation and sometime more if I use the same tool/cutter, every time it involved changing cutter i create a new file for it. It does not mean that somehow Fusion 360 and the post-processor do not issue one by magic??


(William Adams) #17

Here’s the beginning and end of your G-Code:

%
(1001)
(T24  D=0.375 CR=0 - ZMIN=-0.18 - flat end mill)
G90
G17
G20
G28 G91 Z0
G90

(2D Pocket1)
M9
T24 M6
(24)
S10000 M3
G54
G0 X15.5678 Y15.9588
Z0.6
Z0.2
G1 Z0.0994 F39.37
Z-0.0225 F13.12
G19 G2 Y15.9213 Z-0.06 J-0.0375 K0
G17 G3 X15.5866 I0.0094 J0 F100


X8.3734 Y23.4147 Z-0.1613
X8.3704 Y23.417 Z-0.1522
X8.3693 Y23.4177 Z-0.1425
G0 Z0.6
G28 G91 Z0
G90
G28 G91 X0 Y0
G90
M30
%

If you run that through:

http://www.buildlog.net/cnc_laser/cnc/gcode_comment.html

It should be pretty obvious which actions match which codes and which additional behaviors are added by Carbide Motion.


(Alain St-Laurent) #18

Fantastic, “confusion will be my epitaph” (No more).
I did run that html routine, with that translator I guest my next step could be to modify the post-processor, Any advice before a plunge.


(William Adams) #19

My first suggestion would be to check the existing post-processors and see if any offer the behavior which you want.

There should be a list at:

https://wiki.shapeoko.com/index.php/Commercial_Software

Then open up and check out the comments of the ones which seem most promising — usually post-processors are pretty well-commented.

c.f., https://wiki.shapeoko.com/index.php/G-Code#Post_Processors


(mikep) #20

I think your’e trying to make this too complicated.

  1. check the “minimize tool changes” box and f360 won’t put in the tool change…and therefore won’t get CM all confused. This is what confuses the heck out of CM.
  2. One tool per file.