Need Help!- SURFACE ROUGH POCKET

[CNC_BOB]

Hello MCX experts,
I have since MC6 used SURFACE ROUGH POCKET to get things rolling no matter if it is a cavity or boss, but I have always had problems with SURFACE ROUGH RESTMILL to get into areas where the previous cutter could not reach, many wasted moves, aircuts, and even a few nasty pluge moves into solid when there is room for an approach, any hints as to eating out that material would be greatly appreciated, thanks

[Derek Goodwin]

Originally Posted by CNC_BOB Hello MCX experts, I have since MC6 used SURFACE ROUGH POCKET to get things rolling no matter if it is a cavity or boss, but I have always had problems with SURFACE ROUGH RESTMILL to get into areas where the previous cutter could not reach, many wasted moves, aircuts, and even a few nasty pluge moves into solid when there is room for an approach, any hints as to eating out that material would be greatly appreciated, thanks

High speed toolpaths are your friend, try Area clearance and then restmill, it is a different interface than you are used to, but works well, once you have it figured out.

I have videos on the site showing you how to do it, register for the free tour, to view all of the materials, navigate to volume two- High Speed Machining

Mastercam Training Online

[Superman]

Another method is to create an STL file from Verify using all previous operations, and use that fle in place of "all previous ops" or tool size

a lot cleaner and it detects excess material better

another benefit is to use this file as a stock model, to verify the following ops, instead of running all the operations thru verify

[Steve Arteman]

I use stl compare in verify too quickest way to find the leftover material .
Then come up with a plan to clean it up.
Steve Arteman
www.cad2cam.net

[CNC_BOB]

thanks for the pointers, I am trying to save my machined stock as a STL file, I notice that there are tolerance settings, my mastercam is defaulted to TOOL TOLEARANCE .008 AND STL TOLERANCE .001, is this ok? we usually have finish tolerances of .001 total most times. also, when I opened the STL file that I did create, it showed up un-shaded and as a strange looking white wire-frame , still trying.....

[Steve Arteman]

Bob,
You will not be able to shade in the stl file it will however come in as a shaded model in verify when you pick it for the file to use.
What I will do is save the stl for each cut pocket1',pocket2 etc... as the next cut in op manager comes I will use the last stl cut file I stored to verify. This will show a step by step tool by tool toolpath you will see at the machine. In most cases you will not need to do this for each cut but it is really cool when you do need to use it. Stl verify has saved me many times on some of more complex smaller cutter programs. to see where I need to clean up.

Steve
www.cad2cam.net
steve@cad2cam.net

[Mike Mattera]

"my mastercam is defaulted to TOOL TOLEARANCE .008 AND STL TOLERANCE .001"

In Verify these tolerances have to do with the visual representation of the cut part. You know how sometimes the edges of a fine cut might look jagged in Verify? That's what this Tolerance controls. Set it to .0004 and the toolpath verification looks GREAT. This tolerance has nothing to do with the NC Code.

But There Trade-Offs. - It will take MUCH longer to verify the toolpath.

Mike Mattera

[tobyaxis]

Originally Posted by CNC_BOB thanks for the pointers, I am trying to save my machined stock as a STL file, I notice that there are tolerance settings, my mastercam is defaulted to TOOL TOLEARANCE .008 AND STL TOLERANCE .001, is this ok? we usually have finish tolerances of .001 total most times. also, when I opened the STL file that I did create, it showed up un-shaded and as a strange looking white wire-frame , still trying.....

Depend on the accuracy needed you will select the appropriate tolerance of the STL being machined.