Smooth an imported .stp model

[kyp19572007]

I want to ask for help.

The part shown in the image came as a step model and has yet to be modified in Inventor. In the area marked in red (at fillet), many small fragmented surfaces are a problem in CAM design. Is there any way to smooth the surface or to join the many small fragmented surfaces into a continuous surface?

Thanks

[JDMather]

Delete the faces (with Heal) and add the Fillet back in

or

remodel the part from scratch.

Attach your file here if you can't figure it out (preferably the original STEP file).

[kyp19572007]

Well, unfortunately it doesn't work for me (delete face / heal).

Thank you very much for helping.

I attach the original step model.

Thanks,

[WHolzwarth]

This should behave better (2019 IPT).

I've used Construction environment for cleaning.

[kyp19572007]

Thank you very much, but unfortunately I can't open this, I'm using the 2018 IPT.

[Gabriel_Watson · Accepted solution]

This is a great example for the devs (@sundars) of something that should/appears to be an easy change, but Inventor will waste hours of your work trying to solve. Delete with heal failed here at first too, but then I found some leftover (burrs) surfaces on the corners we have to eliminate as well:

     

After selecting those "burrs" on each side with Delete+Heal, the result is a total elimination of the fillet:

If you simply delete those facets and try a boundary patch instead, you end up getting stuck with no way to complete the operation.

My preferred way to fix this is by using the Repair Geometry environment. However, after unstitching the hole solid, deleting all the fillet surfaces and using boundary patch to re-patch the areas (it was a pain to finish these because the automatic edge chain would not work on the blade's side), I still got a resulting multi-face fillet instead of a smooth single-face...

 

[kyp19572007]

Thank you so much for your effort and help!

[cadman777 · Accepted solution]

Find attached my attempt at it using IV2010. I used DeleteFace/Heal and then Fillet w/all the raido buttons checked on the bottom extended panel. My question is, when opened in the newest Inventor are the fillets in this model the same as the OP's or did they become smooth? Here are a couple screen shots of what it looks like as-fixed:

The only thing I didn't like about Heal is it extended the surface perpendicular to the cut instead of along the same contour as the edge. So really it isn't a true Heal.

[cadman777]

I tried remodeling the fins from scratch but couldn't figure it out.

How would you go about doing that since it's complex surface geometry?

[JDMather]

It would take a bit of work and since I don't have 2018...

First I would activate the Construction Environment (Tools Application Options).

Then I would Right Click Copy to Construction.

In the Construction Environment I would set to Feature Priority and move the geometry for one of the fins into separate Groups.  (The cylinders too - but that is trivial.)

Then I would Extract Loops (untrim surfaces) to get to the beginning geometry. 

From there it would be reverse engineering the curves (within any possible realistic manufacturing tolerance - might not be exactly the same to 16 decimal places unless I could figure out how the original designer came up with the curves).

[WHolzwarth]

Oh! After looking at the other files, I noticed, that I patterned five blades instead of initially four ones.

But meanwhile there's enough stuff.

[sundars]

Hi All,

Interesting model. I think the translation of those fillet (blend) surfaces does look bad indeed along with those tiny gaps. On the surface, it looks like those surfaces somehow translated disjoint but they do appear to maintain continuity. I believe we already try to heal it on import but in this case, those tiny faces are not merged back. 

If you look at the fixed up model from @Gabriel_Watson and try to STEP-out the model and import it back into Inventor, those fillets come back in fine.

I would check the original model on the authoring CAD system to see how they the surfaces look like and whether the problem is in the definition of those surfaces or the STEP export operation. 

Thanks

-shiva

[cadman777]

Thanx JD for the steps.

This is where I had problems:

---

@JDMather wrote:

From there it would be reverse engineering the curves

---

I did what you did in in the main editor (not the ConstructionEnv).

But when I duplicated the edges my 3d sketch kept erroring out.

No clue why b/c there was no info from the 'Doctor'.

So I used a Spline connected to the geometry points on the edges and approximated the curvature, then used the top and btm faces of the blade in a Loft with guide rails. It worked. But then when I made a new hub, the fillet errorred out btw the new blade and new hub. No clue why. It will make a fillet of .9mm, but anything bigger fails.

[JDMather]

---

@cadman777 wrote:

Thanx JD for the steps.

This is where I had problems:

….my 3d sketch….

---

I would try to work backwards all the way to a 2D sketch for the foundation geometry.

I didn’t spend a lot of time on this one as I can’t really help get a 2018 solution - but this fin not so complex that I don’t the it could be done relatively easily.  

[cadman777]

Thanx.

No worries.

I did manage to get it done using the ConstructionEnv, but not 'from scratch'.

Thing is, when I export it as STEP, IGES, STL, etc., and open it in Rhino, it shows a mess of RuledSurfaces.

It's even worse than the original!

Thing is, I don't know how the CNC machine will handle it in g-code. But it would seem that if all the fillets are tangent & type Class A, what does it matter that they're constructed in pieces?

[sundars]

Hello All,

I asked our translation team to take a closer look at the STEP file and they confirmed my original thoughts on those blend surfaces being discontinous. It looks like at translation, we split the original blend surface because of several non-g1 discontuinities. At each discontuinity we split the surface and end up with several pieces. While its not ideal, it also helps prevent creating bad bodies. We can certainly take a closer look at the step file and see if we can play around and produce a better model. But ultimately, I would really take a closer look at the original model from the original cad system which produced the step file.

Our internal tracking for this is: ATF-18175.

Thanks and hope that helps.

-shiva

[cadman777 · Accepted solution]

I noticed that Walt.

But it looks even better with 5 blades!