Compensation question

[Stephen]

Hello All,

I have a 3D part that has a couple degrees of taper all around it with blending radi. Basically rectangular in shape. I am using a 1/4" ball nose cutter.

My question is the part did not clean up 100% (Student roughed it undersized if I regen the cutting path but fake out the cutter size with a .235 end mill will it work? Will this give me strange results? Or do I need to scale the part and use the correct cutter size? Finished part size is not critical.

 

Thanks in advance...Steve

 

[ 05-27-2004, 04:01 PM: Message edited by: Stephen ]

[Guest CNC Apps Guy 1]

You can always lie about the size of a cutter. Smaller is usually better if you have to lie.

[mayday]

or leave a negative stock and leave the cutter alone. but be carefull on depths if they are included in the drive surfaces

[kamman25]

make sure you use "comp to tip" if you are trying to hold the depth.

[Jack Mitchell]

Steve,

 

Defining it as a 3D part is not enough a description.

Was this workpiece surfaced or not?

 

If surfacing then correct geometry is required for the cutter – besides, comp didn’t get used.

 

If contouring then yes, cutter radius compensation can be used but this still requires correct geometry for your cutter. I suspect that using a basic square diameter of .250 is the culprit since the issue a drafted cutter with bull nose geometry would require a tool larger than .250 prior to grinding.

 

If a .250 ball nose was used then this would amount to check vs. drive surfacing.

 

You application drawing or the sufaced model would satisfy any query if you upload to Jaysin's ftp site.

 

It still suspect that the student defined the tool as an endmill as opposed to a ball nose cutter.

 

 

Regards, Jack

[Stephen]

Hello Jack,

It was drawn as a solid model. Used surface contour tool path. Comp. was in the computer only. The student didn't leave any stock for roughing and the tool deflected causing the part to go undersize. The finish pass with the ball nose endmill cleaned up 90% of the part. I was just curious what was the best way to proportionally size the part down so we could get 100% clean-up and salvage the part.

 

Steve

[crazy^millman]

Well may not be the best way but might work for you. Xform/Scale then a factor something like .999 or .99 that will reduce the part by a little bit and just regen all of the toolpaths for that section. I am also thinking you might be able to do a negative stock leave amount and that might work but not knowing the part and all of the toolpaths might be a shot in the dark. I hope that helps.

[Thad]

Stephen,

 

You could program it for a .235 ball but run it with a .250 and you'll cut stock.

 

Thad

[Greg Williams]

Hi,

 

I would go with the smaller cutter trick. it works a treat.

I can remember when electrodes were made this way.

[Code_Breaker]

I have used the "lie to MC about cutter's size" when doing electrodes here, and trim tooling at last place I worked. Result were great.

 

I have used scale XYZ on surfaces and it works great.

 

I guess what I am trying to say, there are many ways of doing something, not right vs wrong, but just different.

 

If the finish part size does not matter, experiment with one, then the other and compare the different.

 

HTHAW

HF

 

Code_Breaker

 

--------------------------------------------

X beta tester want-a beeeeeeeeeeeeee

--------------------------------------------