Z Postioning Post Problems?

[Darin]

Hello,

 

I have been having issues with Z positioning on Mastercam.... Maybe it is me.. What is the correct way to chain your geometry.. Have the geometry at the depth of the part or have all chains at Z0? I get confused on the absolute and incremental moves... Here is a example a a simple facing path... I get a weird Z move.. the Only way to get rid of it is to not use depth passes... I have my stock set above for material.... Like my oversize stock is Also I do alot of high end 4th axis trunnion work so I am always checking my Z heights for clearance... Sometimes when I use the same tool for different positions on the 4th it doesn't read the retract Z before the next move...(Equalls crash)... What is the common way to set clearance retract and depth always absolute?

 

 

 

N110 G91 G28 Z0.

N120 (MILLS MATERIAL TO SIZE WITH 3" FACEMILL)

N130 (COMPENSATION TYPE - OFF)

N140 T1 M06 (3" WALTER FACEMILL)

N150 (MAX - Z1.364)

N160 (MIN - Z0.)

N170 M08

N180 G00 G17 G90 G54 X-1.75 Y1.25 S8500 M03

N190 G43 H1 Z1.364

N200 Z.246

N210 G01 X0. F150.

N220 X2.953

N230 X4.703

N240 G00 Z1.364

N250 Z1.246 <--------------------------------- Why this Z move... I only goes away if depth passes are turned off

N260 X-1.75

N270 Z.2

N280 G01 Z.128 F75.

N290 X0. F150.

N300 X2.953

N310 X4.703

N320 G00 Z1.364

N330 Z1.128

N340 X-1.75

N350 Z.2

N360 G01 Z.01 F75.

N370 X0. F150.

N380 X2.953

N390 X4.703

N400 G00 Z1.364

N410 Z1.01

N420 X-1.75

N430 Z.2

N440 G01 Z0. F75.

N450 X0. F150.

N460 X2.953

N470 X4.703

N480 G00 Z1.364

N490 M09

N500 M05

N510 G91 G28 Z0.

N520 G28 Y0.

N530 G90

[kccadcam]

Incremental is the distance from the geometry your driving to, not like G91 incremental on the machine!!!!!

We always use incremental for Feed Plane, Top of Stock, and Depth when possible.

 

 

Try this.....

Clearance is always absolute,

Retract can be absolute or incremental depending on the situation....

[kccadcam]

Sorry,, Retract should have been incremental also in that screen capture......

[NOTW Programmer]

If its 4th axis geometry should be at depth, in other words right on where the features go. My instructor always recomended to use either absolute or incemental, but stick to one only +1 kccadcam incremental is in reference to the geometry; I would have Clearance absolute just so that my tools can retract and approach at the same absolute distancea.

[Mike S @ S4A]

The "extra Z move is most likely from the feed plane - .1 incremental

[K2csq7]

Hi Mike!!!

[Darin]

Sorry,, Retract should have been incremental also in that screen capture......

 

 

Ok I set my setting like yours.... I still get this when it posts.... Even if I set retract to 0 or absolute... Is it a post thing? Again that extra z move only goes away if depth cuts is unchecked..

 

Thanks

 

 

N140 T1 M06 (3" WALTER FACEMILL)

N150 (MAX - Z1.)

N160 (MIN - Z0.)

N170 M08

N180 G00 G17 G90 G54 X-1.75 Y1.25 S8500 M03

N190 G43 H1 Z1.

N200 Z.464

N210 G01 Z.246 F75.

N220 X0. F150.

N230 X2.953

N240 X4.703

N250 G00 Z1.

N260 Z.346 <--------------------------- This move is what I want to get rid of...... Moving up then down real fast scares operators...

N270 X-1.75

N280 G01 Z.128 F75.

N290 X0. F150.

N300 X2.953

N310 X4.703

N320 G00 Z1.

N330 Z.228

N340 X-1.75

N350 G01 Z.01 F75.

N360 X0. F150.

N370 X2.953

N380 X4.703

N390 G00 Z1.

N400 Z.11

N410 X-1.75

N420 G01 Z0. F75.

[Guest]

In depths of cut, have you tried clicking the "Keep Tool down" option?

[K2csq7]

Check the box under Clearance for "use clearance only at start & end of op".

[Darin]

In depths of cut, have you tried clicking the "Keep Tool down" option?

 

 

Here is what the code looks like when I use keep tool down.... Looks like crash to me.. I tried using clearance only at start and end checked and unchecked... Also tried different retract and absolute or incremental... Seams I will have to use ramping to stop the unwanted z moves with depth cuts...

 

N140 T1 M06 (3" WALTER FACEMILL)

N150 (MAX - Z1.)

N160 (MIN - Z0.)

N170 M08

N180 G00 G17 G90 G54 X-1.75 Y1.25 S8500 M03

N190 G43 H1 Z1.

N200 Z.464

N210 G01 Z.246 F75.

N220 X0. F150.

N230 X2.953

N240 X4.703

N250 X-1.75

N260 Z.128 F75.

N270 X0. F150.

N280 X2.953

N290 X4.703

N300 X-1.75

N310 Z.01 F75.

N320 X0. F150.

N330 X2.953

N340 X4.703

N350 X-1.75

N360 Z0. F75.

N370 X0. F150.

N380 X2.953

N390 X4.703

N400 G00 Z1.

N410 M09

N420 M05

N430 G91 G28 Z0.

N440 G28 Y0.

N450 G90

N460 M30

%

[Darin]

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

%

[LaszloK]

I didn't see a crash just an issue with only cutting in one direction. Yor next post with the face mill toolpath cuts in both directions. Can you change the contour path to work in both directions?

[Darin]

I didn't see a crash just an issue with only cutting in one direction. Yor next post with the face mill toolpath cuts in both directions. Can you change the contour path to work in both directions?

 

Well not a crash but it will probably skim the part with no retract at all.. No you can't use contour in both direction with one chain... That is why the face mill operation worked great..