hollow a swept solid 2

[abeschneider]

I am running into a problem when trying to hollow a swept feature. I have basically created a swept feature using a guide string and two end profiles. I want to hollow out the feature, creating a sort of fancy "pipe" (ie pierce 2 end faces and offset the sides). UG NX3 thinks for a while and then says "Cannot Apply Hollow".

Any suggestions? I appreciate it!

 

[feadude]

Does it work if you do not use the offset portion of hollow?

 

[abeschneider]

feadude - not quite sure what you mean. I have tried (1) specifying the ends to pierce AND the sides to offset (2) spec just the ends to pierce and neither method works. Note that the "Hollow" command requires a value for "default thickness" and an optional "Alternate thickness". I've tried both (+) and (-) values for these. My tolerance is set to 0.0254. Any ideas?

 

[feadude]

I usually do not use the alternate thickness because I have not used the offset faces yet. I though if you hollow all the same thickness it might work. It is possible that hollow (offset) faces are moving in different directions and software can not connect them together.

 

[abeschneider]

hmm, I should have been more clear. I've never mixed (+) and (-) default and alternate thicknesses - I've tried both (+), both (-), and also leaving alternate thickness off.

 

[cowski]

For starters, I would examine the swept to make sure all the geometry is valid, solid and curves (Analysis -> Examine Geometry... [NX2 location others may vary]). If that checks out ok, try plan B -- extract body your swept feature (make sure 'at timestamp' is checked) then try to offset the extracted body and subtract that from the original.

If the geometry is ok, but won't offset then that means that the offset (or hollow) operation would cause something to become invalid. In that case you probably need to tweak the original swept geometry.

Hope this helps.

 

[abeschneider]

I will try what cowski recommended...

One more thing. My section profiles are rectangular. I've noticed in playing around with a couple simple examples (trying to understand why I'm running into problems) that offsetting of rectangular sweeps seem to magnify surface irregularities. This doesn't seem to be an issue with smooth circular swept features...

 

[cowski]

Rectangular sections, now I understand and feel your pain.

If you do Information -> Object (face subtype) and mouse over your solid, you probably won't see what you expect to. It is my experience that a rectangle will end up with 2 faces around the perimeter rather than the expected 4. Two 'corners' get converted to a very small radii which makes it nearly impossible to offset.

If your section stays constant along the guide you might try the 'sweep along guide' feature (not the freeform 'swept' feature), it doesn't take as many liberties with your input geometry. If you need the power of the freeform 'swept' feature (it can cause headaches but it really is a powerful command), you might try blending the corners of your section geometry by at least the value that you plan to offset the surface.

 

[abeschneider]

hehe I thought something was fishy here! I looked closer at my profile sections, and a possible source of the problem is that instead of rectangles being made of 4 edges, my rectangles had 6 line segments (I had used a mirror command to make the rectangle). I altered the profiles so they were made of 4 lines, and then I was able to get the hollow to work, but so far, only with (+) value of offset. I actually need to use a (-) offset, so I'm still chugging away.

Couple more details: My part is very large (ie XS area = 7m^2). W/the default hollow tol. value of .0254, I had weird "bubbly" surfaces on part of the model. Tightening the tol. to .00254 seemed to correct this.

I'm going to try blending the corners like cowski suggests. (I need to use the "Swept" feature, because the cross sectional area changes over the length)

Thanks for all the replies

 

[cowski]

One more alternative is to model the 'inside diameter' (I realize the cross section is rectangular, but I couldn't think of a better term) then do the extract body, offset the faces of your original feature out the material thickness and subtract the extract body from the swept. Drawback to this method is if you plan to blend edges along the tube later you will run into trouble.

 

[abeschneider]

I appreciate your ideas...all I can say is this has got to be one of the most frustrating features to work with in NX3. It's so difficult to use "Hollow" on rectangular cross-sections, that I'm about at the point of just not hollowing at all.

I did find that another alternative is to create 2 sets of profiles; representing the inside and outside of the tube. Then "Swept" both of these, and do a Boolean "Subtract" operation to effect the hollow. All these procedures are compute-intensive though, and take a long time to refresh...

 

[cowski]

I've been through this before and I finally remember the trick! In the swept dialog (not your global modeling preferences!) set the tolerance to 0. This will keep the hard edges as hard edges and will allow the hollow operation to work.

 

[abeschneider]

COWSKI!

that last tip - setting the "SWEPT" dialog tolerance value to "0" works!

Also, it works quickly, without too much CPU time to compute.

THANK YOU very much. A star for you!

 

[HellBent]

cowski's tip is a good one....you're not the first to get frustrated with the sweeps.
The most important thing to try to do though is keep your section strings consistent from end to end. Think about what the software is trying to do when it's making that sweep. It's trying to transition from one section to the next and needs good definition to do so. Try to maintain the same number of points, lines, etc. whenever possible to make it easier for the software to determine the path of least resistance. The best example of this is sweeping a rectangular section to a circular section. If you try to do it just by drawing a box at one end and then a circle at the other it won't work. But if you break the circle up into 4 segments corresponding to the sides of the box and select start points that relate to one another it will do the sweep just fine. All it needed was some help determining what points to use.

Take care....