Concave corner

[Alexanders]

I'm using a simple path for contour milling with compensation for tool wear.
KeepOffsetsMMFanucComp.set

Code: Select all

%
N100 (COMPENSATION-WEAR)
N102 (TOOL 1 - DIA 10.  mm)
N1 G90 G17 G40 G80 G00 
N103 M06 T1 ()
N105 G00 G54 G90 X15.145 Y221.578 S3183 M03 
N109 Z9. 
N110 G01 Z0. F668. 
N111 G41 D1 Y221.577 
N112 X246.474 
N113 X230.631 Y-5. 
N114 X-5.362 
N115 Z9.
N120 M30 
%

However, even with the smallest negative correction value, an error occurs: "Concave corner with cutter radius comp". The angle between the lines is 86 degrees.
Other CNC systems follow this trajectory with negative correction, without error messages.
I've tried adding small arcs to the corners, and it works. But it doesn't suit me. What can I change in the settings to prevent this message from appearing?

[TomKerekes]

Hi Alexanders,

That would be technically incorrect and is difficult to implement because one block of motion can't be determined until the following block of motion is known. Block 1's motion can't be determined before Block 2. Also if Block 1 or 2 consists of multiple small blocks the result is somewhat indeterminate.

gouge.png (5.49 KiB) Viewed 22020 times

Your example of 86 degrees isn't really relevant is it? Any angle less than 180 degrees would cause gouging correct?

Which CNC systems support this?

Why doesn't adding arcs suit you?

One workaround might be to create the GCode slightly undersized such that all corrections would be positive. Would that work for you?

If you really need this to be added would you be willing to fully test it? There would be a number of special cases. Single stepping would execute delayed. A embedded MCode between compensated moves would either need to execute before the last motion or otherwise allow a gouge.

[Alexanders]

Your example of 86 degrees isn't really relevant is it? Any angle less than 180 degrees would cause gouging correct?

This is a real example from the machine's operation. Part of the above program that is not executed and causes an error.
This is contour milling of sheet material.

Test1.PNG (6.45 KiB) Viewed 21969 times

One workaround might be to create the GCode slightly undersized such that all corrections would be positive. Would that work for you?

This is a bad path. Other program elements do not allow this.
The designer develops a G-code program using the CAM system. The CNC operator executes this program using only a cutter wear correction.

[TomKerekes]

This is a bad path. Other program elements do not allow this.

I don't understand what you mean.

But I think all the issues still exist.

Neg Offset.png (11.15 KiB) Viewed 21963 times

Zoom.png (8.08 KiB) Viewed 21963 times

Could you answer my questions?

[Alexanders]

I'm sorry for the long answer.

Why doesn't adding arcs suit you?

Because the product should have a sharp corner, without a radius. The products has a variety of geometries, and manually adding arcs is not advisable. This will increase the possibility of errors in the geometry. In addition, it will significantly increase the design time.

Which CNC systems support this?

Here are examples of running the same program in LinuxCNC:

Zero tool compensation:

Positive tool compensation:

Negative tool compensation:

No concave angle errors occur.


I'll also remind you of the question I asked earlier. These are additional cells for correcting the instrument's compensation. This is very convenient and reduces operator errors.

AddOffset.jpg (9.82 KiB) Viewed 21936 times

[Alexanders]

Is it possible to make the trajectory work like in LinuxCNC ?

[TomKerekes]

Hi Alexanders,

We were looking into it. But it difficult and has the drawbacks I mentioned.

I don't understand the need.

Why doesn't adding arcs suit you?
Because the product should have a sharp corner, without a radius.

With an arc less than the tool the corner will always be sharp.

The products has a variety of geometries, and manually adding arcs is not advisable. This will increase the possibility of errors in the geometry. In addition, it will significantly increase the design time.

Aren't you using CAD? It should add the arcs without possibility of error.

[Alexanders]

Aren't you using CAD? It should add the arcs without possibility of error.

Many models with complex geometry and many concave corners per day.
Adding multiple arcs makes the process infinitely long and often leads to other errors.

I have tested this and similar programs on Fanuc and Haas CNC systems. They and LinuxCNC do not cause concave angle errors and perform the path correctly with any tool compensation values.

[TomKerekes]

Many models with complex geometry and many concave corners per day.
Adding multiple arcs makes the process infinitely long and often leads to other errors.

Could you explain? Are you using CAD?

ChatGTP thinks Hass does not allow it:

Official Reference: Haas Alarm 367

The Haas Alarm 367 – “CUTTER COMP INTERFERENCE” is documented in multiple technical references. It states:

Alarm: 367 CUTTER COMP INTERFERENCE
Description: Programmed path cannot be computed with tool size. Use a different size tool or adjust the radius offset.
CNC Cookbook
+13
Helman CNC
+13
Practical Machinist
+13

This clearly indicates that when the tool radius prevents the controller from calculating a valid offset path—such as in a sharp concave inside corner—it will stop and signal an alarm, rather than try to “make the best of it.”

Community Confirmations

While Haas documentation isn’t always explicit about concave corners and interference behavior, machining communities consistently observe this behavior in practice:

On forums like PracticalMachinist, a contributor notes:

“If you have radii that get smaller than the amount of compensation… Program cannot handle that.”
Practical Machinist
+1

This supports the idea that the control recognizes when a tool offset is physically unachievable and responds with an error.

Summary

Yes, when the tool’s radius makes a sharp concave corner impossible to follow with G41/G42, Haas will raise a Cutter Comp Interference alarm—it does not cut as close as possible or "trim” to fit the corner.

To avoid this alarm, the solution is to either:

Use a smaller tool,

Modify the programmed corner (e.g., add a fillet ≥ tool radius),

Or have your CAM generate a compensated path that stays within viable geometry.

Its difficult but we may look into it. You didn't answer if you would be willing to test. Would you ?

[Alexanders]

Are you using CAD?

Yes, Solidworks and Solidcam.

ChatGTP thinks Hass does not allow it:

ChatGTP, like other AI systems, is often deceptive. I have personally tested this program on Fanuc and Haas CNC milling machines. There are no concave corner errors.
The CUTTER COMP INTERFERENCE Alarm has a different meaning. This means that after G41/42, the path from the start point of the tool compensation is less than the radius of the tool. This is a very useful warning, but it has nothing to do with a concave corner.

You didn't answer if you would be willing to test. Would you ?

Yes, I'm ready to test. What should I do?