chamfer problem 1

[MickyV007]

Hello,

i'm trying to create a chamfer on a half hole (see part) and it keeps giving fault errors. I can create a blend but that's not what i need.

Any suggestions or ideas would be very appriciated!

Using NX 4 (but tried it in NX6 also with no succes)

Thank you on forehand.

Greetz Michaël

Michaël Verheyen
CAD designer
PHILIPS INNOVATIVE APPLICATIONS N.V.
Belgium

 

[potrero]

Michaël,

You can easily do what you're trying to do. Here's how I'd do it:

1. Assuming you want to place a chamfer on either the elongated slots in the small diameter cylinder, or in the "half hole" where the coned body meets the smaller cylinder, first step is to Split Bodies. (Insert > Trim Body > Split Body). Select the solid body, and Split it with the XC-YC plane. Now you should have two Solid Bodies in your part file.

2. Now create your chamfers as you normally would.

3. If you want, boolean Unite the two bodies back together again.

Hope this helps.

 

[morans]

Michaël, potrero's idea will work, but will leave you with a non-parametric solid. Depending on the application, this may or may not be acceptable.

Another way that you could do it is to extract the edge curves of that particular hole, then create a sketch to sweep it along a guide (the edge curves you extracted). Whatever sharp ends or corners that might be left over can be trimmed with a datum plane/trim body before subtracting it from the main solid.

this will leave the model 100% parametric hope it helps. I wasn't able to open the file you attached as we're still using NX3/NX4 here

 

[MickyV007]

First of all thank you potrero for the fast response,

but i still did found another solution, and well for two reasons :

1) If i use the trim body function i lose all my parameters, which is not so nice if you need to change something afterwards.

2) I got some strange triangle cut out in the Yc-Zc plane from the hole.

If you look at the model you could see my solution, putting some parameters on the sketch and you can create the chamfer you want.

Still wonder why the chamfer function would not work?

Kind regards,

Michaël

Michaël Verheyen
CAD designer
PHILIPS INNOVATIVE APPLICATIONS N.V.
Belgium

 

[mmauldin]

Potrero's approach can be kept parametric if you mirror the body about the X-Z plane, then trim the two bodies rather than splitting the original body. Using this method left a small "undercut" in the tapered bore.

I took an approach similar to morans', but used an extrusion with a draft angle to create a solid which was then trimmed and subtracted. This left no "undercut".

 

[MickyV007]

Mmauldin,

i indeed fell over the "undercut" and the parametric issue, and took a different approach though than you without the trim body function,but with the same result.

Still got the feeling that the solutions are all kindalike work arounds.

Best regards and thanks for responding,

Greetz,

Michaël Verheyen
CAD designer
PHILIPS INNOVATIVE APPLICATIONS N.V.
Belgium

 

[hudson888]

Michaël,

I have put together three results that help to illustrate the problem and a possible parametric solution I think it is equivalent to what others have done, anyway.

The problem in your case is that the taper in the hole differs from the sides of the slot. It means that you end up with an odd extra face in the corners that the system could not resolve to create on its own.

You can create a subtraction solid of the correct geometry and then not trimming the sides of to get the extra face see where the problem lies, that compares 0002321_a.prt with 0002332_c.prt which is very similar to what potrero did.

The other version just 0002321_b.prt just illustrates why a blend worked and how to hatch a cunning plan to duplicate that result with a chamfer like effect.

Best Regards

Hudson

www.jamb.com.au

Nil Desperandum illegitimi non carborundum

 

[JohnRBaker]

OK, try this approach out for size.

The scheme I used is based on an old trick that has been around for years where you simply use a 'Blend' as a sort of 'skeleton' from which you can then construct what you need to create a sheet body which represents the face of the 'Chamfer'. Once you've got the sheet body, simply use it to trim away what was the blend. Note that if you wish to edit the size of the Chamfer, simply edit the size of Blend(17).


John R. Baker, P.E.
Product 'Evangelist'
Product Design Solutions
Siemens PLM Software Inc.
Cypress, CA

http://www.siemens.com/plm

http://www.plmworld.org/museum/

To an Engineer, the glass is twice as big as it needs to be.

 

[JohnRBaker]

Opps, I forgot to attach the part file. Here it is.

John R. Baker, P.E.
Product 'Evangelist'
Product Design Solutions
Siemens PLM Software Inc.
Cypress, CA

http://www.siemens.com/plm

http://www.plmworld.org/museum/

To an Engineer, the glass is twice as big as it needs to be.

 

[hudson888]

John,

It tends to Self intersect though so I did a version with a ruled surface using Arclength alignment which you can just patch on and Michael can compare it with the earlier blend derived example that I did. The two surfaces yours and mine are still in the file so you'll see the shape changed partly because when I sought to take the self intersection out of the corners of course the internals maps themselves differently and result in s different shape. I hope that it makes sense in some small way.

Best Regards

Hudson

www.jamb.com.au

Nil Desperandum illegitimi non carborundum