Defining a chamfer cut

    
  Subscribe Topic

Rank: 1

OldForumPost

Newbie

posts: 0

Registered: 2012-1-14

Message 1 of 9

 Defining a chamfer cut
05-07-2007 11:22 . am   |   View his/her posts only
I'm working on a part that required a series of slots and v-notch cuts. It is really a simple part that should just require a couple repetitive 2-D operations. But for the v-notches, I need an angle cutter. I tried defining and modifying various tools, and eventually found that only one that would work was a chamfer cutter.

I was able to define the chamfer feature in my CAM plan, using the bottom edge of the notch. But when I generate the tool path with a 2 1/2-axis chamfer operation, everything is off-set by over an inch. I've tried adjusting everything I can think of in the parameters, but without any luck. I also had some luck using the same tool with a 2 1/2-axis chamfer operation using slot feature, but this also seems rather erratic.

Am I on the right track, or is there another way of doing this? I'd be grateful for any suggestions.

Thanks,

Daniel

Rank: 1

ChrisWard2k2

Newbie

posts: 2

Registered: 2011-11-22

Message 2 of 9

05-07-2007 02:02 . pm   |   View his/her posts only
Hi Daniel

Your description makes perfect sense to you because you are familiar with your work in-hand, but I'm not really sure how your geometry shape looks.........a file would be useful. The CAM cutter does of course need to be representative of the tool you will actually use (at least in most cases). A simple profile feature should provide the containment necessary but without actually seeing your geom, there is not much help to offer you.

Rank: 1

OldForumPost

Newbie

posts: 0

Registered: 2012-1-14

Message 3 of 9

05-07-2007 02:48 . pm   |   View his/her posts only
Thanks for the reply. I tried attaching the VX file and a screenshot of the geometry with the first posting, but I guess it didn't work... I'll try again here. The part 'Distributer - tube' and the 'Distributer - tube CAM plan' are the relevant parts of the .vx file.

Rank: 1

ChrisWard2k2

Newbie

posts: 2

Registered: 2011-11-22

Message 4 of 9

05-07-2007 05:54 . pm   |   View his/her posts only
Hi again Daniel

Well, it is complex depending on the engineering requirement. The tool you defined, 90 degree chamfer of zero diameter, might be hard to find Not sure that this is really a job for a chamfer operation (you have not specified the material). The notch is 0.30dia, that could possibly be cut out with a counter-sink op, before the slot is cut. Since you have a 3-axis, the lead-out face from the notch could then be produced with an end mill. The slots are only 0.08 (2mm) wide but your 1/16 end mill could do that?

Requirements are key (especially tolerance of course) - it will be near impossible to cut the notch accurately without a blemish on the face of the slot. If the design can be changed, have the slot slightly deeper than the notch. If this part was a component for a mold tool I would not think twice about using an electrode to produce the shape since an electrode would be easier to machine.

Run Solid Verification on the attached file and see if this leads to an inspired solution.....

Update: If you can get hold of that chamfer cutter, the attached method might work for you.

Rank: 1

Jianxin

Newbie

posts: 0

Registered: 2002-10-17

Message 5 of 9

06-07-2007 09:45 . am   |   View his/her posts only
Hi, Daniel:

If you really want to use your milling cutter, please define a profile by picking
the bottom lines and use 3x surface engraving to cut those lines directly.
To have the correct cutting direction, pick the bottom lines one by one and
then reverse their directions.

In the operation form, choose "Pick Order" to machine and input proper
approaching and retracting data. The approach and retracting heights can be
changed by editing "Main Frame."

Please use "Vertical Thick" to manually adjust the cutter along z-axis. Check for
reference the attached file which was saved in 12.86.

Jason

Rank: 1

OldForumPost

Newbie

posts: 0

Registered: 2012-1-14

Message 6 of 9

06-07-2007 10:04 . am   |   View his/her posts only
Chris - Thanks for the reply. Seeing your CAM plan was very helpful; using the profile cut and engrave cut worked great. I had not been using profile features, and those certainly make things easier.

The material in this case is plastic (PVC), so I think I'll be able to get by without the drilling operations. The tolerances also aren't too tight - the angle cut feature is just to provide a perpendicular surface for the small (0.030") holes that are later drilled in at 45 deg.

I've got the CAM plan for a single tube as it should be, but was hoping to make a single CAM plan for the assembly, which includes two of these tubes (also included in the distributer.vx file I uploaded). When I try the same operations on the assembly, they don't work. Am I missing some trick for assemblies with multiple identical components? When I select a feature on one part, the corresponding feature on the other part is also selected -- which might be part of the problem...

Thanks,

Daniel

Rank: 1

OldForumPost

Newbie

posts: 0

Registered: 2012-1-14

Message 7 of 9

06-07-2007 10:27 . am   |   View his/her posts only
Jason - Thanks for the tips. I had not used the surface engrave operation before, and it definitely helps out. It is nice to have the extra control over the exact path of the tool. I checked out the parameters you mentioned, and am still exploring it...

Daniel

Rank: 1

ChrisWard2k2

Newbie

posts: 2

Registered: 2011-11-22

Message 8 of 9

06-07-2007 10:39 . am   |   View his/her posts only
Hi Daniel

There is a good way to cover the requirements of CAM, which are different of course to those of CAD. It would be nice for example to have the Z direction of the Target Part match CAM Z, thus reducing the need to define alternative CAM Frames and probably helping one to visualise the machine set-up better. The way to do this is to create a new Part Object specifically as the CAM Target Part. Use Insert Component and Merge to bring-in the Model. Now you can orientate the model to suit CAM, add containment features, drill points etc without messing-up the design data - but if the design data changes, this CAM Target Part will update too. The Merge should break the associativity that the Assembly is holding for CAD purposes, so you can then treat each tube as a separate un-linked entity.

Rank: 1

OldForumPost

Newbie

posts: 0

Registered: 2012-1-14

Message 9 of 9

06-07-2007 02:01 . pm   |   View his/her posts only
Chris - I tried it again with the components merged and it all seems to be working. So I'm all set to generate code... Thanks!
See also
X