machining help

[perseid88]

We are primarily a drill and mill shop but today I have a different task that I need help with.

 

I need to surface mill a 5° bevel on the end of a part (carbon steel). We are only talking a few square inches but I don't know how to program this.

I have uploaded a yolk.dwg file (not the .dxf version, it can be deleted) of our part to the drawings folder of the FTP site. Each end (top and bottom) has a 5° slope to it.

 

I was thinking we would use a ball (bull?) end mill but I don't know what sort of toolpath will do that angled surface.

Up to this point, all of my programming has been limited to 95% drill with some pocket and contour.

Am I creating the angled surface and milling with some sort of stepdown to the prescribed angle or depth? or ...?

I guess I could buy a special flat end mill with a 5° angled bottom but we'd rather not.

 

Phil

 

[ 04-15-2010, 04:16 PM: Message edited by: perseid88 ]

[jeff]

I haven't seen the part, but I would probably go with a Surface/Finish Flowline if you have mill 3

 

Edit:

I think all you need is Mill 2 for finish flowline, but can only do 1 surf at a time.

[jeff]

I would use a bullnose personally, but a ballnose is equally good.

Depending on the finish quality desired, you can use something like a 3/8 dia tool, 8,000 rpm, 75 ipm with a .004 stepover.

Just for starters and tweak from there

[perseid88]

I think your edit is correct because when I try surface/finish/flowline, I get the error that I don't have that in mill 1 and I need mill 2.

 

Goes to show yo how much straight drilling/milling we do. I never needed mill 2 before.

 

Any other options with mill level 1?

 

Phil

[perseid88]

Ok, so I botched the bull vs ball term. No quarter for a newbie, eh? I can take it.

 

With the .004 stepover, what

type of toolpath are you suggesting will do the variable depth?

[Matthew Hajicek - Singularity]

You should be able to do it with a "wireframe" toolpath in Mill 1.

[Santa Fe]

Just draw two lines parallel to each other with the 5° that you need, then choose toolpaths/wireframe/ruled, then select the two line described above, select your tool (the 3/8 ball will work fine) adjust feed and speed, go to ruled parameters and select zigzag, across distance use about .010 to start, set comp in computer to "off" and set the tip comp to "tip" that should do it for level 1 licence.

[3R!< W3NG3R]

I would try wireframe sweep.

[Cad-Camr]

You can do this with a 2d contour cut with a bull nose or Ball end mill if you have enough clearance. Select the geometry at the bottom of the angle and in the depth cuts enter the angle in the tapered wall box and your step over in the depth cuts. You can use a square ended tool also but that requires a smaller step down to get a good finish. I like to use a Bull Nose with a small radius then I dont have to go to deep to get the tool tangent. You may have to move the geometry out and down a little (X 5 Deg) so the radius of the tool clears the bottom of the part.

[MotorCityMinion]

Is it a straight or curvy edge that is uniform in width throughout it's depth? If so, just use the taper function in 2d contour. Play with it as it's easy to figure out.

[perseid88]

Thanks all. Some of the suggestions above didn't provide the intended results or ended in an error somewhere.

It was the process from Santa Fe that got us to where we wanted to be.

Thanks also to my Mastercam rep who chimed in w/ a private message and offered to help.

[Goldorak]

use wireframe swept 2D in mill 1

 

easy efficient and simple to use

 

if you want it one way instead of zig-zag , run swept2R.dll c-hook

[bigjohn]

Or you can use a macro program.

 

 

.