PDA

View Full Version : 3-D milling with BobCad



outback
02-15-2015, 05:19 PM
Has anyone used BobCad to machine a part like this? I have
BobCad V25 for milling but have never used it, long story.

http://img.photobucket.com/albums/v30/jglass/Shop%20Demonstrations/CAD%20Drawings/tail%20plate.jpg (http://smg.photobucket.com/user/jglass/media/Shop%20Demonstrations/CAD%20Drawings/tail%20plate.jpg.html)

All I need to machine is the raised area on the one surface. How difficult is it to get BobCad to write a CNC program for this job?

Thanks,
Jim

Rich Carlstedt
02-15-2015, 09:50 PM
Perhaps posting this question on the Digital Thread here will yield more info ?

http://bbs.homeshopmachinist.net/forums/9-Digital-Machinist

Rich

elf
02-16-2015, 12:37 AM
You can to do that with 2.5D, which BobCad should be able to do with little effort.

Black Forest
02-16-2015, 10:32 AM
I am curious as to what tool you would use to machine the two slanted faces? Assuming using CAM software and coming in with the tool perpendicular to the bottom flat face. Maybe a ball mill?

George Bulliss
02-16-2015, 10:37 AM
I am curious as to what tool you would use to machine the two slanted faces? Assuming using CAM software and coming in with the tool perpendicular to the bottom flat face. Maybe a ball mill?

Ball end mill would be best, the bigger the ball, the larger the Z-step you can use without sacrificing the finish. If the radius between the flat and the feature is small, a end mill with a corner radius (bull nose) will work. Stepping down is fine for roughing, but for finishing with a ball end mill, going from the bottom up will give a better finish.

Black Forest
02-16-2015, 11:13 AM
Danke!

lakeside53
02-16-2015, 11:29 AM
Ball mill.. But it's a lot quicker to do a tool change and put a 45 degree face mill in and plow both sides (or just do it for "finishing" passes) . Better finish too.

DR
02-16-2015, 07:35 PM
You certainly can do it with a ball end mill. But, you'll get a scalloped surface. Tilt the part and do the angled surface with a square end mill.

Another way, if you have the tool, use a 45 degree tapered cutter.


To the original question...quite easy to generate code in CAM. (Easy for me to say 'cause I do it all the time.)

outback
02-16-2015, 08:46 PM
Thanks for the replies. Originally I was thinking of using a 1/2" ball endmill. But now I think I can cut
the angles by simply tilting the workpiece in a vice. The workpiece is for a steel guitar and not particularly fussy. The piece is only 5" x 5" square.
Thanks,
Jim

Black Forest
02-17-2015, 06:57 AM
Outback your part is finished. I cut it out of steel. Of course this is no help to you regarding BobCAM but it was an exercise for me.

I am trying Autodesk Fusion 360 and decided to model and setup the model in the cam and do a simulation of machining the part. I used a 10mm endmill and a 4mm ball endmill. One roughing pass with the ball endmill and then a finish pass. The finish pass is shown in brouwn.

http://youtu.be/fL6-Oa6aTjo

George Bulliss
02-17-2015, 07:38 AM
Black Forest, in my earlier post about cutting from the bottom up with a ball end mill for better finish, that was for the finish pass only, cutting maybe .005"-.010" at most. The main shape is typically roughed out using larger bull nose or flat bottomed end mills from the top down.

Black Forest
02-17-2015, 09:36 AM
Black Forest, in my earlier post about cutting from the bottom up with a ball end mill for better finish, that was for the finish pass only, cutting maybe .005"-.010" at most. The main shape is typically roughed out using larger bull nose or flat bottomed end mills from the top down.

Now you tell me! Did you look at the video I posted?

outback
02-17-2015, 09:37 AM
Just had a thought. If I supplied a Solidworks model of this part could someone here write the program?
My CNC mill runs on Mach3. This part will probably require some rounded edges not shown on the picture posted. I'm on vacation in Florida. The job was emailed to me from a regular customer. Don't have all the details right now but I know I'll get the job.

After 10 years of cnc machining this is the first job that requires 3D machining. I would hate to spend time and money learning BobCad for what could be a one time job.
Jim

George Bulliss
02-17-2015, 10:12 AM
Now you tell me! Did you look at the video I posted?

Yes, saw the video and just looked again, see you changed it up a bit. Agree with others that tilting the part and cutting the angles that way is probably best for a one off part. My following comments are based on what I would do for a similar looking mold component in a commercial shop, where you always want to limit the setups. Machine time is cheap and you can be doing something else; flipping the part around takes money. Not saying this is the only way, or even the best way, it's just one way. Finish and size requirements might not call for as much monkey business. Of course, the home shop is a whole different ballgame...

Let's assume it's okay and desirable to leave a 1/8" radius at the base of the standing V. I would do a pocket (or clearing, or whatever your system calls it) toolpath with a large bull nose end mill, leaving about .010" stock on X and Y and on the Z flats. Either add the 1/8" rad to the model (best) or use a cutter with a nose radius of 1/8" or greater. Start at the top and don't get too wham jammy in your Z cuts; you don't want huge cusps interfering with the following cutters.

Once the part is roughed, finish the Z flats with a flat or bull nose end mill, keeping away from the radius. Run the pass a little high, check dimensions and run again to finish on size.

Next, I would run a semi finish program (ball end mill, same size as finisher) on the standing part and start at the top, leaving .002". After that, change to the finisher ball end mill and start at the bottom and step up, climb cutting.