Question about lofting techniques (probably) 3

[Heinrich3333]

I`m a relatively new user in NX, so please bear with me.

I`m modeling a valve housing, as shown in the attached sketches.
The inner extruded feature has a height ("diameter") on 122 and the half-circles on the top and the bottom are size R25, the hole on the outside has a diameter of 95. What I want is to create a constant angle in the area with height difference between the inner and outer feature, marked with a red ring in one of the pics.
I`ve tried numerous more "solidworks-y" ways to try and achieve this (trying to directly extrude between to different profiles on different sketches, for instance, and extruding with draft), but I finally find myself stuck with no satisfying way to accomplish this presumably simple task.

Any input would be appreciated.
-Henrik

 

[Heinrich3333]

Apparently I could only post one file at a time. Here is the one referenced in the post.

 

[JohnRBaker]

First off, if you wish to include more than one file, simply zip them up and upload the .zip file.

As for your model, it would be much better if you could provide an actual part file, not necessarily all of it, but at least a chunk of it where this 'passage' is being created. Also, what version of NX are you running?

John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Industry Sector
Cypress, CA
Siemens PLM:
UG/NX Museum:

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

 

[Heinrich3333]

Right, the history is a bit messy, but what the hell, here is a part of the housing.
The passage I speak of is the passage where the circles extruded on the sides "meet" the half-circles (on the up and downsides) of the extruded figures on the inside. Instead of the height difference I want a constant angle from the inside and out to the face of the structure.

 

[JohnRBaker]

Are we talking about something like the green face in the attached model?

John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Industry Sector
Cypress, CA
Siemens PLM:
UG/NX Museum:

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

 

[Heinrich3333]

Thank you for your reply.
We`re closing in, but even so the optimal design would be if the shape was a constant R25 half-circle going with a constant angle out from 122 mm to 97 mm.
Is that even possible?

-Henrik

 

[SiW979]

Is this what you are looking at? It's a bit rough, but with a bit more time it could be made to work. From feature 76 onwards.

Cheers

Si.

Best regards

Simon NX 7.5.4.4 MP8 and NX 8.5 (native) - TC 8 www.jcb.com

 

[SiW979]

This is a much cleaner solution.

cheers

Si



Best regards

Simon NX 7.5.4.4 MP8 and NX 8.5 (native) - TC 8 www.jcb.com

 

[SvenBom]

OK, here is mine, with Throug Curve method.
When you'll open my model, check the following:
1. your extrude(42) is suppressed
2. i have added a Datum plane to the position, where the end of your extrude was. This is the expression named, depth.
3. on that plane, I have drawn the Sketch(44). Check that sketch. You can see, that there are three dimension. Arc_radius is set to 25. Arc_distance is ste to 97. Slot_positoin is half of the arc_distance.
4. With ThrougCurves command, I have connected your sketch with mine.
5. With Subtract command, I have made this opening.
Now, if you want to change the dimension, the easiest way is to go to Tools/Expression and search for the four dimensions, I have mentioned before.

I hope, that this method will help you.
Regards.

 

[Heinrich3333]

Hey you guys, and thank you for all the interesting replies.
I tried going forward with SvenBom`s method because it looked easy, and I think I`ve got what I need. Even so, stars for everyone!

Again, thank you all very much!
-Henrik