What's new
What's new

Cutter Comp issue on Doosan Mill with Fanuc Control

Matthewkral

Plastic
Joined
Jul 21, 2021
Hello guys.

I am using a dovetail cutter to mill both sides of a male dovetail feature. I am cutting roughly .015" too much on both sides. I used Gibbscam to program this. The largest diameter on the bottom of the dovetail is 2.25". I have a .25" line and a .25" radius entry move into the workpiece and am starting way off the part for clearance. I am climb milling and using G41.

I entered a positive .015" radial offset to move away from the workpiece and cut .015" larger on either side. It is not alarming out, but it is not comping and continues to cut the same size. What might cause this? Could it be that my entry moves are too small? Is there something else I should look for?
 
It might help to post your code and describe the size of the dovetail cutter, and if you're programming to the part edge or using an offset path. Yet without seeing anything, the easiest thing would be to add another 0.015" to your D comp entry. That's the beauty of using cutter comp. Not cutting the correct size? Change the comp setting. No re-programming needed.
 
It is not alarming out, but it is not comping and continues to cut the same size. What might cause this?
Calling up the wrong D value, or you entered the .015" into the wrong D location.
OR
Or you're D callout is in a previous portion of your program and the control hasn't processed it. This could happen if you're restarting past the D callout.
 
It might help to post your code and describe the size of the dovetail cutter, and if you're programming to the part edge or using an offset path. Yet without seeing anything, the easiest thing would be to add another 0.015" to your D comp entry. That's the beauty of using cutter comp. Not cutting the correct size? Change the comp setting. No re-programming needed.
Here is the generated code. I am using an offset path so that (theoretically) I don't need to start with any sort of comp and the cutter should cut where I want it to given everything is perfect. I did add .015" to my D comp entry and no changes were made.

N4T4M6( TOOL 4 - 2.25 HSS DOVETAIL 45 DEG )
G17G80G40
G0G90G54X-1.625Y.57S1500M3
G43Z2.H4M8T5
Z.1
G1Z-.5F50.
G41Y.32F3.D4
G3X-1.375Y.07I.25
G1X5.875
G3X6.125Y.32J.25
G40G1Y.57
G0Z.1
G0G90X6.125Y-3.97
G1Z-.5F50.
G41Y-3.72F3.D4
G3X5.875Y-3.47I-.25
G1X-1.375
G3X-1.625Y-3.72J-.25
G40G1Y-3.97
G0Z.1
M9
G0G91G28Z0.
 
Calling up the wrong D value, or you entered the .015" into the wrong D location.
OR
Or you're D callout is in a previous portion of your program and the control hasn't processed it. This could happen if you're restarting past the D callout.
I've replied to another comment with the code.
 
N4T4M6( TOOL 4 - 2.25 HSS DOVETAIL 45 DEG )
G17G80G40
G0G90G54X-1.525Y.32S1500M3
G43Z2.H4M8T5
Z.1
G1Z-.5F50.
G41X1.625F3.D4
G3X-1.375Y.07I.25
G1X5.875
G3X6.125Y.32J.25
G40G1X6.0
G0Z.1
G0G90X6.000Y-3.72
G1Z-.5F50.
G41X6.125F3.D4
G3X5.875Y-3.47I-.25
G1X-1.375
G3X-1.625Y-3.72J-.25
G40G1X-1.5
G0Z.1
M9
G0G91G28Z0.


Suggest perpendicular comp moves into your lead-in arc.
 
Here is the generated code. I am using an offset path so that (theoretically) I don't need to start with any sort of comp and the cutter should cut where I want it to given everything is perfect. I did add .015" to my D comp entry and no changes were made.

N4T4M6( TOOL 4 - 2.25 HSS DOVETAIL 45 DEG )
G17G80G40
G0G90G54X-1.625Y.57S1500M3
G43Z2.H4M8T5
Z.1
G1Z-.5F50.
G41Y.32F3.D4
G3X-1.375Y.07I.25
G1X5.875
G3X6.125Y.32J.25
G40G1Y.57
G0Z.1
G0G90X6.125Y-3.97
G1Z-.5F50.
G41Y-3.72F3.D4
G3X5.875Y-3.47I-.25
G1X-1.375
G3X-1.625Y-3.72J-.25
G40G1Y-3.97
G0Z.1
M9
G0G91G28Z0.
What is stored in D4? (Both geometry and wear values)
What is the cutter dia?
 
He is comping in a line tangent to the arc he wants to cut. I’m guessing the control can still successfully complete the arc even though the starting Y is slightly off.

I bet if he puts a large amount into his comp he’ll get an alarm.
 
Part of the op's problem is the dovetail cutter being used is likely oversize as most HSS milling type cutters are. Unless it was measured carefully, over-cutting using a nominal offset could be expected. And 15-30 thou over wouldn't be unheard of.

Still doesn't explain why when he adds comp it doesn' seem to change things. If I'm not mistaken, seems to me there's a parameter that sets whether the control will alarm out or not when it detects an over-cutting situation or too large of an offset number. I may have that wrong. My memory does that... :-)
 








 
Back
Top