Problem: Carbide Motion did not prompt to change cutters

Hello all,

The problem I am having is that Carbide Motion does not prompt me to change the cutters. Instead, it continues to operate with the first cutter (which happens to be a 0.25" face mill).

My set up is as follows:
iMac 27-inch Mid 2011 / 8GM memory / 3.1GHz Intel Core i5
Fusion360 CAM
mach3mill.cps post processor
Carbide Motion version 2.0.314 (2015-04-09)

I have attached some illustrative images for reference.

Any help would be very much appreciated!


Carbide Motion paused after not prompting to change cutter:

Fusion360 CAM setup showing the different cutters assigned to each operation:

Nomad883 paused after beginning to cut the next operation without prompting to change the cutter:

This is a snippet of the G code:

(T1 D=0.25 CR=0. - ZMIN=0. - FACE MILL)
G90 G94 G91.1 G40 G49 G17
G28 G91 Z0.

T1 M6
S12000 M3
G0 X2.3292 Y-3.3036
G43 Z0.85 H1
G1 Z0.27 F20.
G18 G3 X2.3042 Z0.245 I-0.025 K0.
G1 X2.1667
G17 G2 Y-3.0679 I0. J0.1178
G1 X2.1667
G3 Y-2.8322 I0. J0.1178

[continues the face milling operation]

G1 X2.1667
G18 G2 X2.1917 Z0.15 I0. K0.025
G0 Z0.85

[right after the face milling operation is complete, it continues the next operation without prompting to change the tool—why?]

G0 X-1.7123 Y-2.4435
G1 Z0.1313 F20.
G19 G2 Y-2.4498 Z0.125 J-0.0063 K0.
G17 G3 X-1.706 Y-2.4561 I0.0063 J0.
G1 X-1.6681
X-1.6647 Y-2.4562
X-1.6407 Y-2.4569

Did you check the “Manual Tool Change” checkbox on the “Post Processor” tab of the tool setup in the tool library? Also make sure you give the cutters unique numbers in that dialog as well.

From the screenshot it looks like all of your tools are listed as #1 and that is definitely a problem.

Here is an example of a tool library when it is set-up for multiple tools. Notice how the CAM operations are listed under each tool that is used from the library?

1 Like

I believe I have found the solution.

Problem: Carbide Motion did not prompt me to change the tools (i.e., cutters).
Solution: Name each tool (cutter) a different number and select “Manual Tool Change”.

To clarify, all of my tools were labeled #1 as pictured below.

This made Carbide Motion think I wanted to continue using the same tool, since the tool number did not change.

To fix this, I did the following:

  1. Navigated to [Manage > Tool Library]

  2. Changed the tool numbers (and, while I was at it, chose “Manual Tool Change”).

  3. Reassigned the tools to my operations.

  4. Output my post processing code again.

  5. Called myself a stallion in the mirror and ate a cookie.

1 Like

Yes! I had discovered this while digging around in Fusion 360. Then I took twenty minutes to write response before noticing your solution.

Your reply was much more concise than mine. Lol.



1 Like