Simple facemill opperation with contour

[Darin]

Hello,

 

 

We do alot of facing material to size with various face mills 1.25" to 4.0". The operators would like a simple path over the material with depths cuts cutting in both directions.... So come down to a depth mill in one direction (Left/Right) of the material then move down to next depth and feed the other direction (Left/Right).. I use to be able to program like this in SmartCam years ago.. How can this be done with Mastercam. They would like these to be part of the program instead of hand editing this move at the machine or have me edit it in the code.... We do to much of this at different depths and different cutters... I came close with ramping and unchecked one way ramping in closed open contours...

[Matthew Hajicek - Singularity]

Use the "Face" toolpath, it will do that. You can set style to "One Pass" if the cutter + overlap > stock width. You can either chain a rectangle for your stock, or not chain anything and have it use your stock definition. Then give it depth cuts and set the top of stock and cut depth appropriately and you're set.

[Cannon]

I came close with ramping and unchecked one way ramping in closed open contours...

 

Change the ramping motion to plunge, it will feed to next depth of cut at both ends of your chain, so just chain one side of you part or draw a line in the middle of part and set the compensation off.

[Oscar R.]

If it's a single pass on the face of your stock at each depth that you want, just use the Face toolpath set to "one pass" on the style. In your depth of cuts set it as you would like and check the "keep tool down" box.

That will give you on pass at each depth in both directions.

[Darin]

Use the "Face" toolpath, it will do that. You can set style to "One Pass" if the cutter + overlap > stock width. You can either chain a rectangle for your stock, or not chain anything and have it use your stock definition. Then give it depth cuts and set the top of stock and cut depth appropriately and you're set.

 

 

Great thank you... Worked perfect..

 

 

I use face mill tool path and these setting with depth cuts worked perfect.... Seams weird though that I couldn't get the contour to work...

 

 

 

N100 G00 G17 G20 G40 G80 G90

N110 G91 G28 Z0.

N120 (FACEMILLS WITH 3.0 FACEMILL)

N130 (COMPENSATION TYPE - COMPUTER)

N140 T1 M06 (3" WALTER FACEMILL)

N150 (MAX - Z1.364)

N160 (MIN - Z0.)

N170 G00 G17 G90 G54 X-1.8 Y1.25 S8500 M03

N180 G43 H1 Z1.364

N190 Z.464

N200 G01 Z.246 F75.

N210 X4.753

N220 Z.128

N230 X-1.8

N240 Z.01

N250 X4.753

N260 Z0.

N270 X-1.8

N280 G00 Z1.

N290 M05

N300 G91 G28 Z0.

N310 G28 Y0.

N320 G90

N330 M30

%

[Cannon]

If it's a single pass on the face of your stock at each depth that you want, just use the Face toolpath set to "one pass" on the style. In your depth of cuts set it as you would like and check the "keep tool down" box.

That will give you on pass at each depth in both directions.

 

I never knew I could get it to machine both ways, learned something new today! Thanks!

[Oscar R.]

I never knew I could get it to machine both ways, learned something new today! Thanks

No problem. Glad to help.

[Matthew Hajicek - Singularity]

The "keep tool down" works nicely in zigzag too now; it no longer picks up and goes back from whence it started but merely turns around and retraces it's steps at the next depth.

[dylskee]

I never knew I could get it to machine both ways, learned something new today! Thanks!

 

+1

Man, learning the little things really help!