[riverracer]

hi guys, i'm having trouble getting a cavity to cut properly.
(proberly newbie errors)
have done it as a surface revolve, (should it be from a solid?)
the top dia was on size, the next dia was 0.15mm over size.
and the both depths were 0.2mm shallow.
1st i roughed it with a 'surface rough pocket' with a 16mm dia x .8r, 1mm stepdown and 0.5 stock left.
then used 3 'surface fin contour' with a 14mm dia x 0.5r.
1st was the top flange, 0.1mm stepdown.
2nd the next dia with 1mm stepdown. (as this dia gets thread milled)
finally the taper and rad with a 0.1mm stepdown aswell.
it also left a step between the 2nd opp and the bottom taper.

its a simple job, so what am i doing wrong?

can i tell it to use 'control' for the cutter size, instead of setting the size in the tool pram?

(the blue lines are the containment boundrys, these and the dim's are on different levels)

X4 MU3 with solids

thanks

[Matt Berube]

No, there's no advantage to using a solid for this feature. I prefer to always cut surfaces on 3-D toolpaths due to occasional errors I've had working directly on solids.

I can't understand why you would have surfaces on size or oversize if you specified .5 stock to leave on drive surfaces. That should never happen.

Perhaps you created the operation using a "bull mill" (corner rad) but then cut the part with a sharp cornered end mill ? This would likely cause the issue you experienced... It's hard to say without actually looking at the operations you created...

If you want to hit depths accurately in roughing you need to specify the depth in the "cut depths" area of your toolpath. I am fond of using Absolute depths. Min/Max should be obvious and for any intermediate steps you need to press the "select depths" button and select some geometry on screen for the desired depths. Otherwise, Mastercam would just divide the cut into equal depth cuts which usually results in varying amounts of stock left on the part.

If you need more help than this I'd recommend uploading your file again including the toolpaths you created and then perhaps we can be of better assistance.

[cadcam]

Well I just opened your file and no paths so I can not review what you have done.if you share that file I might be able to review and update it for you.
I just got done programming these little molds for production on a Horz cutting up to 250 IPM and the part comes in with in .001 on the CMM. So most likely there is an issue with the surface or the settings in most case's or the strategy used.


I also cut from the solid 90percent of the time and do not have issues.I know Matt B is a Great programmer and knows his MC , But I do not agree with always changing to surfaces.

Cheers Matt.

[Matt Berube]

Hi Cadcam,

Thanks for the kind words. The only reason I prefer surfaces is due to a few frustrating errors I've experienced in the past where cutting on the solid produced scrap but creating surfaces from that same model produced good toolpaths. This probably only happens on 1 in 1000 models.... Maybe even less frequently... But when it absolutely positively has to be right the first time I prefer surfaces.

Happy Easter everybody.:cheers:

[riverracer]

hi guys,
sorry been off computer for easter hol's, and now will try again.
sorry bout no cutter paths, looks like i zipped the wrong file.
have applied the same paths i used before, but to a solid this time.
(feeds and speeds not set yet)
roughed out with a tipped 20mm x 0.8r cutter. (1) within 0.5mm dia.
finished with a 14mm x 0.5r cutter. (2,3,4)
(2) 0.1 stepdown, flange 2mm deep.
(3) 2mm stepdown, as this area gets thread milled.
(4) 0.1mm stepdown on taper.
still getting the step at the bottom/start of the taper.
the only way i can seem to get rid of it it to combine the 3rd an 4th opp into 1.
but this would take a long time at 0.1 depth cuts.

am i using the wrong toolpath types?
can you pls show me where i am going wrong.

X4 MU3 solids

thanks again

[Matt Berube]

Operation #4 needs more drive surfaces to keep from gouging the vertical wall. You only selected the tapered face and the small radius at the bottom. Adding the 51mm cylindrical face as a drive surface will prevent the gouge however it will be cutting more than you desire because you haven't restricted the "cut depths" enough. Change the MIN cut depth to -26.55 and you should see a suitable toolpath.

To avoid problems with gouging in the future I recommend selecting all of the surfaces and/or solid faces as "drive" and then restricting the toolpaths as necessary with cover surfaces, boundaries, and/or depth limits. The only time I don't select all faces as drive would be when the model gets large or complicated enough that toolpaths take too long to calculate and then I need to proceed with caution. At least 90% of the things I toolpath use all faces for "drive".

Hope this helps.

[riverracer]

thanks matt,

picked the sidewall aswell, reset the cut depth limits and it looks ok.
also cured the bore oversize problem !

you guys are great for us newbie's.

:cheers: