Haas controller tool to big error

[ftporta]

Hello All,

Just reworked a Haas VF-OE that I've never used so far with Fusion 360.  When I post out a test program that works fine in the Fusion simulation, the controller on the Haas returns a "tool too big error" (error 369) when it tries to machine the second op.  The second op is a 2D contour finishing operation around an island using cutter comp.  Specifically, the control stops execution and highlights line N10000.  The NC file is attached, as well as a screen cast of the test part that was posted out.  Does anyone have any ideas? 

Thanks in advance.

[daniel_lyall · Accepted solution]

There is a lot of posts online with that error http://www.helmancnc.com/haas-alarm-369-tool-too-big/   what is D1

[engineguy · Accepted solution]

@ftporta

Hi, it looks like you have a D1 tool offset call that is moving the tool offset from the CAM software to the machine control, check in the machine control what the tool offset #1 is set to, not sure if it is the same in the HAAS as other controls but most have an offset amount for wear/actual size that is a very small value, often the actual diameter or radius has been input by mistake making the tool "Too Big" for the cut to be made.

Anyway, I am with @daniel_lyall with this, the D1 would appear to be the culprit, also you could try setting the "Compensation Type" to "In Computer" just as a test as that should not generate the G41 D1 line of code and see if the error clears at the machine.

If you can please upload your .f3d as it does make it easier for folks to look for errors, thanks

Regards

Rob

[ftporta]

Yes, I changed D1, and finally got the alarm eliminated.

Thanks Daniel.

[ftporta]

Rob,

You and Daniel were correct.  I finally got back to the Haas VMC yesterday, and reduced D1, and the controller executed the program.  I appreciate the help.

best regards,

Frank

[daniel_lyall]

Sometimes the second and 3rd look are needed to find a silly little problem glad it is sorted.

[markEJ3EB]

Where or on what screen do you go about changing D values? On tool offset page? 

[programming2C78B]

Yes. The tool Dia should 0 on the controller (offsets page) and then use In Computer or Wear in fusion.