not so simple edge blends 4

[opetrenko1]

For two days I've been struggling to blend couple of edges show here in orange

We need about R0.5" on the "airfoil" and anything around R0.1-0.3 on the plate.
I hoped to do it in a couple of robust parametric features, as this to be replicated 20-30 times on other similar geometries.

I also tried face blends. But, when I'm trying to put a through curve mesh where blends meet at the leading edge, I get strange error "cannot sew sheets"

Attached is the part in NX6. (I can borrow NX8.5 devl license, but we don't have nx9 yet)
any ideas are greatly appreciated.

 

[jerry1423]

Here is my best attempt.
You may want to step thru the features to see how I did it.
The suppressed bottom features are yours that you had on there.

 

[jerry1423]

Here it is

 

[jerry1423]

Sorry but mine was saved in NX7.5.

 

[JohnRBaker]

Do you have the original model with all it's features? I ask, because this 'body' has some serious topology issues! Remember, "You can't make a silk purse out of a sow's ear."

That being said, I did manage to get you something which might meet your needs. I first ran it through the 'Heal Geometry' utility which did clean-up some of the topology issues, at least enough so that I was able to get a fully blended result.

As for the workflow, use Edge Blends whenever possible. Don't use the 'Tangent Curve' rule for models like this, it's better to select your edges one at a time, so set the rule to 'Single Curve'. Start with the small blend on the 'plate' (the biggest I could go was 0.2"). Then add the larger 'airfoil' blend. Work on one side of the model and then the other.

Anyway, take a look at the attached model and see if this works for you. BTW, I did it all in NX 6.0.

John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Industry Sector
Cypress, CA
Siemens PLM:
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To an Engineer, the glass is twice as big as it needs to be.

 

[JohnRBaker]

That was an awfull lot of effort jerry1423 and while you got it to blend, I suspect that it was all for naught since I think your assumption that the airfoil was symmetrical was incorrect.

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.

 

[jerry1423]

I just took maybe 10 minutes to do that . . . sorry but I thought it was symmetrical.

 

[JohnRBaker]

Perhaps not in time, but certainly in terms of the number of different operations performed.

In my example, after cleaning up the model using the 'Heal Geometry' utility, it took only 4 simple edge blends. Granted, you had to be careful about the order of creation and how you selected the edges, but the final result is as simple as it could possibly be, and the original asymmetrical shape is preserved.

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.

 

[opetrenko1]

Jerry and John, thank you!!!
Jerry, that's very tricky use of Replace Face.
Face Blend continued with an edge blends is even more. How none of them work by themself but their combination works so nice? Symmetry is not an issue, as I know now how to do it. Thanks!

John, Amazing how simple your solution works after healing. It will take me a while to sanitize the parametric part. Let me try to debug the issue first. Could you point me to where did you notice the topology problems? The design of this blob was quite a puzzle to me. I made it with a pile of features. I'll try to tigten the tolerance and check the contstaints. How would you model such an airfoil blob attached to a random sheet? Trailing edge shape is nonimportant.

Again, thank you very much!

 

[jerry1423]

my blending took 6 features, yes 50% more than what you required, but not too bad.

I am a bit of a "replace face" nut. It has been part of NX (and Unigraphics) for something like 23 years, and have always had fun with it.

 

[JohnRBaker]

If you run Examine Geometry on your orginal model (after deleting everything but the solid body) you'll see some tolerance problem areas. After creating a 'cleaner' model using the Heal Geometry utility, while there are still some problem areas, they are reduced. The biggest problem that I saw when I first looked at the model was that extra 'edge' along one side of what you called the 'plate'. That should not be there and doing a 'Join Face' did not remove it (another tool to help clean-up model topology, or at least simplify it).

Now as for your comment about tightening modeling tolerances, please don't go overboard. Higher (i.e. Smaller) tolerance values does not automatically mean higher quality or even better precision. I say this despite the fact that for NX 9.0 we have tightened (made smaller) the, out-of-the-box, default modeling tolerances as set in Customer Defaults. Prior to NX 9.0, the default Modeling tolerance for Imperial unit parts was 0.001 inches and for Metric it was 0.0254 mm. Starting with NX 9.0 that has been changed to 0.0004 inches and 0.01 mm respectively. Of course, we still recommend that users take into account the overall size of what their products are in determining what a reasonable tolerance setting might be. For example, if you design cruise ships versus watches, you wouldn't expect to use the same Modeling tolerance values now would you? And just to put the new settings into perspective, the values now being used are what is generally accepted as the industry standard by the automobile manufacturers and their suppliers, who now makes up the largest portion of our customer base, which is what motivated us to make this change to our OOTB defaults. The previous values were based on a time in our past when aerospace was our largest market segment, albeit when we were also a much smaller company with nowhere near as many customers as we have today.

As for what are good modeling practices for the design of airfoils, I have no direct experience in that area as I'm an old machine designer who spent 14 years working in the R&D department at a large multinational supplier of capital machinery to the food and chemical processing industries.

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.

 

[opetrenko1]

John,
for some reason when I increase blend radius even by 0.01" to 0.21" the other blend - last one - fails. How would you debugging this when I ran into some errors making the rest dosen of parts?
May be even more general question to you and Jerry: where do you even start learning troubleshooting these wicked tricks, with replace face and combining edge and face blends? I ran "examine geometry" and got all tests passed with tolderances from 0.25deg / 0.00005" to 0.5deg / 0.001"

As for original shape this isn't some specific NACA airfoil, just a drop-like shape with a trailing edge made of 2-3point splines. Even its general size is very approximate: "about this tall (shown with fingers), about this wide and about this long". So, it's a general shape that was difficult for me to construct (and impossible to blend).
Thank you for helping me out

 

[jerry1423]

Where did I learn the tricks ?
Mostly from just playing around the last 25 years on NX (and Unigraphics).
The nice thing about NX is that the more you know about it, the more you appreciate it . . . and the more fun you have with it.

 

[JohnRBaker]

That last blend, that's the one on that face with the seam (extra edge) down the middle. It's possible that that's what's messing with that blend because on the other side, where that is a nice clean face, you can increase the radius to 0.3 inches.

And again, as cowski said, practice, practice, practice, and I've been using NX (Unigraphics) for going on 37 years.

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.

 

[cowski]

And again, as cowski jerry1423 said, practice, practice, practice

Fixed, but I do agree.

www.nxjournaling.com

 

[mcwickham]

Hi John,

Any idea why the change to the default model tolerance is not mentioned in the release notes for NX9? or am I just missing it?

Matthew Wickham
Product Data eXchange
Delphi

 

[JohnRBaker]

They are documented in the NX 9.0 Release Notes at:

Home -> NX 9 Caveats and Product Notes -> CAD -> Modeling -> Product Notes

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.