Undercutting 1

[sekhon]

Can anybody tell how to do undercutting with lollypop tools in NX3?I can't make the tool to reach undercut area while finishing.I know this can be done easily on mastercam but I couldn,t find any way to do that on NX3.Any help will be greatly appreciated. Thanks

 

[HellBent]

hmmm..I haven't done any programs with a barrel cutter but assumed if you defined your tool as a barrel cutter it would recognize where the shaft dia. was and be a breeze. Did you define the cutter that way? Interesting timing though...I've got some cylinder head programs to write in the next week or so and may be dealing with the same issue.

Take care....

 

[sekhon]

Yes I tried to define a tool but didn't work at all.

 

[wmalan]

You stated it didn't work at all... Could you be more specific? I've done this a lot.

What type of operation are you trying and how is it setup. Boundary or Surface Area? Surface Drive tends to work the best. For a test - don't select Part - only the Drive Surface and see if you are getting something. Also, make sure your Drives normal is pointing out. Engage, Retracts are towards and away from the surface to clear the part.


--
Bill

 

[sekhon]

Hi bill,
I am trying fixed contour and I am selecting faces.I can post me part on this forum but I don't know how to do it.I tried to define a barrell cutter as lollypop cutter but nx is cutting the part only upto the edged of the flutes not upto the edges of shank as it's shank is less than the cutter.Please reply me if can find some way out. Thanks.

 

[wmalan]

Here's the simple way (but it only cuts one face):
Use Fixed Contour/Surface Area and select one face as the Drive Surface. Don't select Part or Check at this time. It should be working now. It may gouge the surrounding faces but at least your moving forwards here <g>.

For mulitiple faces (and no gouging) you'll need to use Surface/Boundary or Surface/Drive. Boundary will require bounding geometry that is projected towards the cut. The boundary must be large enough or minus stock to allow the tool to fit "thru it".

Drive of course requires a drive surface but you might be able to use the actual cut faces*. Select either the whole part as "part" or just the immediate faces which is what I usually do to avoid unnessesary calcuations.

*I say might because UG expects the Drive surfaces to be "contiguaous". Many times your dealing fragments of faces.

A lot depends on the situation especially the acuteness of the undercut.

Any better?

--
Bill

 

[sekhon]

Hi bill,
Thankyou for providing me helpful hints.I tried as you suggested and it worked.I used 2 ways:

1.Fixed contour-surface area as a drive method. in this method I can machine only one face at a time.But I got so many tiny surfaces.Is there any way to select multiple faces at a time like selecting faces in area milling?

2.Second I tried was Fixed contour-boundry as a drive method.In this first I extracted all edge curves from the faces i want to machine and then selected those curves as a boundry.I had to change the plane of boundry too b'coz undercut is facing +Y axis.So I selected +Y axis plane and I selected Y axis as a projection vector for boundry and It worked. Now there are some questions rising in my mind:

1. what if my workpiece is round and undercut face is round too.It worked in previous piece b'coz it was facing Y axis.

2.When I tring to verifing it it's showing gouges.I thing it's showing gauges b'coz ug assuming barrel cutter as a straight ball nose cutter.If I look at the toolpath it doesn't looks like gouging.
Thanks again for replying!!

You can check my part here:

http://sekhon.photosite.com/Album1/cavity.html

 

[wmalan]

From your pics I can assume your simply entering into that cavity like a boring tool would from the side? If that's the case, I'd just use PlanerMill using Profile with "Direct" moves between passes so the tool does not pull up after each pass around the bore. Much easier to control.

--
Bill

 

[sekhon]

I think I can't use planer mill b'coz it's not an even profile.I added 2 more pics and it will make more clear to you what area I am machining.It will show tool path too.Could you please have look. Thanks

 

[wmalan]

Now I see. Use Fixed Contour. Select the Part surfaces to cut. Select the left edges (or extract and create your own) as an "Open" boudary for the tool to follow. Have the tool engage at the bottom of the cavity then drive up the edges with multiple passes.

That should do it!

--
Bill