[PhoenixMetal]

Hi, I am relatively new to Mastercam and was hoping you can help. I am using Mastercam's High Speed Machining Area Clearance Roughing toolpath to clear out a large angled surface. The tool I am trying to use is a 3" indexable carbide facemill (the tool is capable of ramping). I just got the tool, but from my initial experimentation with it, I can only run it at a depth of cut of 0.006". Much more and either the spindle stalls or it breaks an insert.

My problem is, that when I set the Z stepover value to 0.006", Mastercam takes an extremely long time to calculate the toolpath, since it is calculating a million little passes. I haven't yet gotten it to calculate completely as after the 45 minute mark, I've gotten disgusted every time and restarted the program.

Am I doing something wrong? Should I be using a different toolpath for roughing with high feed / light depth of cut tools?

Thanks for your help.

[Steve Arteman]

Is your problem on the plunge that you can only take .006 depth cut? is this a blind pocket to rough out or can you use the side of the cutter to lead in to a cut? if so try surface rough pocket. it is hard to tell with out looking at the part.
steve
www.cad2cam.net

[kesparate]

there are hardware concerns to consider here. master cam is very powerful, and it munches computer resources to accommodate. if you're trying to create a tool path like this that's going inches deep in .006 steps that is one hell of a lot of math, and if your pc isn't up to snuff it can take hours to calculate. i think steve might be on to something. is this really the best strategy?

[PhoenixMetal]

Thanks for your help - I got it to work acceptably - I changed up my parameters to use a much lower feed per tooth (and therefore a slower feedrate), which made it possible for my machine to handle a much larger depth of cut of 0.1". This more normal Z depth is a whole lot less taxing for my computer to crunch than the 0.006" I was using before. The new toolpath takes only a few minutes to calculate.

Thanks for your help guys.

Now that the machine is happily cutting away, I'd really like to optimize the toolpath. The HSM Core Roughing toolpath (sorry I incorrectly stated that I was using Area Clearance earlier) is spending a lot of time cutting air. Definitely more time cutting air then cutting metal. Here's a picture of what the toolpath looks like:



I don't understand why its spending so much time away from the material, and if it was going to be away from the material, should it be moving a faster rate to reposition? I do have Tool Containment set to Outside, because otherwise the (3" diameter) tool wasn't able to cut the far extremes to the left and right of the part. I have containment set to a 3D chain that starts at the close left at the beginning of the ramp and goes uphill, downhill, over (away), uphill, downhill and over (towards you) again.

Is there a different toolpath I should be using or a different containment strategy that would keep from cutting air so much?

Oh, to give you an idea of scale for the workpiece, it is approximately 4" wide x 3" tall x 0.75" thick, and is hardened 4140 steel.

Thank again for your help!

[timmydabull]

to eliminate the cutting of air you will need to trim your toolpath(s)

trimming toolpaths are accomplished by creating wireframe geometry around your part and using that geometry to tell your tool if you are outside of this boundary rapid to new cut position.

this functon is enabled by clicking on
toolpaths
trim toolpaths
select operations to trim
select trimming wireframe
select which side of the wireframe to trim to

hopefully this will help.

[cadcam]

you are not using the tool correct these are entry and exit high speed moves if you trim the tool path then DO NOT use this path. please share the file so we can show you a betterway to cut this.

thanks cadcam

[Superman]

Have you selected the entire solid as drive or check surfaces, try using the minimum required
Mastercam will check the tool and path to all your selected surfaces (both drive and check).

Do you think there may be a more efficient stategy to use ?

These 2 may give a better result
1/ Rough Flowline - use the 2 angled faces and the top radius as your drive surfaces
2/ Rough surface project- similar to #1 but uses a curve projected onto your surfaces to define the toolpath line ( like a 3D facing operation along your curve only ) , only use Z positve moves, from both sides

[PhoenixMetal]

Hey Guys thanks for your help! I have attached the MCX file for your reference as CadCam requested.

You have prompted me to realize a critical activity within Mastercam that I have so far gotten away without doing (struggling however) for the week or so I have been using the software: That is drawing geometry specifically for the purpose of containing toolpaths.

Since I am working exclusively with imported Solidworks models, I skipped out on learning to draw geometry in Mastercam - but now I realize that instead of just selecting geometry that is already in the model for driving and containing toolpaths, I can actually make new geometry for this purpose.

Thanks for your suggestions on the better toolpaths.

[cadcam]

I am sorry what version of Mastercam X are you using I will be opening with X3 MU1?

[cadcam]

Here is the part cut with the angle. This part was a 2d profile not a 3d part.
this needed to be put back laying down and cut.
Review file and picture.

[PhoenixMetal]

Cadcam, thank you so much for taking the time to rework the part file! It was very instructive to see how you did the contouring in three steps: Two for roughing just the corners off, and a third for following the actual curve.

However, I have a question: I noticed the first contour operation you had it set to leave 0.4" in XY broken into 3 passes, and the second contour operation you had it leave 0" in XY broken into 2 passes. Why did you break it into two operations instead of one single one to leave 0" in XY in 5 passes?

Thanks again!

For anyone else who is interested in opening the file, its an X3 file.