Surface-Rough-Pocket

[scooch8292]

I am using Version 9.1 MR0105 and am having issues with my surface-rough-pocket routines. I would like to leave stock on the sides of the pocket but not the bottom. I have the cut depths set to absolute and have detected the flats. The "Adjust for stock to leave box" is not checked as the help screen says not to, to machine to the depths I have selected. Any one else having these issues or know a way to rough these pockets to the correct depths????

[Jim at Gentex]

Welcome to the forum scooch8292!

 

 

Did you try using absolute depths with min / max values instead of incremental depths w/ adjustment to top cuts? This has always worked for me.

 

edit:

OOPS...Just reread your post and see you did try absolute depths...sorry.

 

You may consider separate toolpaths for the sides and bottom to get what you need.

[JohnA]

Scooch,

I presume this pocket is not a typical box. If the walls and the floor of the pocket are all the same surface then I don't think you can do what you are wanting to do. You may be able to split the surface and make the floor with a small amount of the wall a seperate surface,then run your surfacing operation on the wall portion with stock-to-leave and on the floor portion with 0.0 stock-to-leave. Let me know if I'm even close as it's been awhile since I've done this.

JohnA

[mayday]

stock to leave includes all surfaces. run a secondary surface path to finish the bottom by selecting the sides as check surfaces and setting stock to leave on the check. or set up a boundry chain to stay away from the sides. the adjust for stock to leave setting in depth cuts only means the the depth cut z moves are adjusted to take in acount for the amount of stock your leaving

[deeherk]

welcome to the forum scooch!!!!!

dan

[gcode]

If your surfaces are not too complex you can lie to Mastercam. Define your 1/2in endmill as .560

dia and set stock allowance to zero.

Use a real 1/2 endmill when you machine the part.

You will have zero on the floor and .030 on the walls.

If you're using a bull endmill you'll need to lie about the tool radius as well if you are machining

horizontal or nearly horizontal surfaces

[scooch8292]

Thanks everyone for you idea's and comments. Yes this part is not a typical box. It has many differet levels inside the pocket I did end up lying to Mastercam and telling it that the roughing tools were bigger dia by twice the stock to leave I wanted. It doesn't verify properly but it'll get the job done the way I want to. Thanks again!

[Thad]

Scott,

 

I've seen this before. It has been logged by CNC Software as bug #3990.

 

Welcome to the forum!

 

Thad

[scooch8292]

I brought this issue up with our Mastercam supplier about 3 years ago and they said I/Mastercam couldn't do that either and to rethink my machining processes. Maybe Version X will solve that prblem for me then. Thanks for the input.

[Müřlıń®]

quote:

---

If your surfaces are not too complex you can lie to Mastercam. Define your 1/2in endmill as .560

---

+1 to Gcode.......do this all the time But with extremely complex surfaces also....

 

OPS definition example:

 

1.0" ball T1

1.03" ball T100

 

Makes the NC file easy to edit