Cannot place fillet

[Anonymous]

I cannot place a fillet on the outside or on the inside of the back of this part. Whether I

use extrude, or boundary patch then thicken Inventor says the part is too complicated.

This is my first real go at surface modeling and I must have done something wrong at the

closed end of this part.   What should I do to this part to allow the fillets to be created?

Thanks, Don

Autodesk Inventor Professional 2014 SP2

64 bit Edition

Windows 7 Professional SP1

Dell Precision T3500

Intel Xeon 3.07GHz, 12.0 GB

[TheCADWhisperer]

Did you attach the correct file here?  (the file I opened does not look like the image that you attached)

If you do a Manage>Rebuild All do you get any errors?

[Anonymous]

Yes, That file is the exact file it has only been renamed. I opened it and did the rebuild all and received no error messages

but still no fillet.

[ASchlaack]

Here is what I'm getting when I download the file you posted... It is definitely not what is shown in your image, plus it has errors.

[ASchlaack]

Sorry, the image didn't attach to my last post.

[Anonymous]

That's Interesting, Maybe its because you are opening it with Inventor 2016. I created it in 2014.

It looks like the move face operation failed.??

[TheCADWhisperer]

Can you save the file as a STEP (*.stp) and attach here.

Sometimes a Face Fillet will work where edge fillet fails.

Frankly, I think I would model the part quite differently, but I am not sure where you are going with the design.

[Anonymous]

If I suppress the Move Face1, I get a failure of the boundry patch4 and Sketch 28, Now my part looks exactly like the image you posted.

Does this mean I need to start over on this part?  I agree that this should be modeled differently but Im not sure exactly how. I will post the

STEP. I am having trouble with posting the STEP. Please rename the extension to .stp and then try opening it.

Thanks for your help

[ASchlaack]

2017 actually, but that shouldn't cause an issue, it should be able to migrate into 2017 just fine. But I guess it's a possibility if you can open the same file just fine.

Sorry I couldn't be more help.

[Anonymous]

Actually you were a help. When I converted the file to STEP, I was able to place the fillets on the outside

and the inside no problems. Now the part is exactly what I want. The problem is when I need to change it.

Thank you Aaron

[johnsonshiue · Accepted solution]

Hi Don,

This is a very interesting case for surface modeling. I have been taking a look on and off and I think I have found a good solution. First, profile and rails have G0 continuity (non-tangent). If I were you, I would fix them up. They will cause trouble down the road. Second, the key to have a good guide rail sweep here is to create a good 3D rail. Here is what you need to do.

1) Delete almost everything in the part and leave Path, Rails, and Profile sketches intact. Fix up the tangent issues.

2) Create a 3D Sketch -> Intersection Curve -> pick one of the rails from Rails sketch and pick the path -> Ok. You will get an intersecting curve as if the two surfaces extruded from the sketches individually.

3) Guide Rail Sweep -> pick the two profiles -> pick the curve in Path sketch as path -> pick the intersection curve as guide rail -> Ok.

You will get a pretty even sweep. The surface quality will be very good and the geometry is unnecessarily complicated. Downstream features will not fail as a result. Try it out and let me know if it works for you.

Many thanks!

[Anonymous]

Hi Johnson,

                It seems the 3D sketch > Intersection Curve gives a very smooth transition without all of the surfacing patchwork.

You are correct G0 continuity on profile and rails. I think that's because they were both projected geometry from the mating

parts.

               I don't know of a better way to get the G1 continuity required other than 1. Project geometry, 2 Click on the 54 nodes

with fix constraints one at a time and delete them, and 3. Add the tangent constraints and hope the sketch does not distort in the

process.

Thank You for looking at this and for your suggestion. It works much better this way, I will continue to work on this.

Thanks again

Don

[johnsonshiue · Accepted solution]

Hi Don,

Many thanks for the confirmation! The geometry is much smoother and clean (not unnecessarily complicated; sorry for human multi-threading error!). The reason why the intersection curve works better here is that the Y-direction profile scaling is in sync with the sweep path. The original guide rail was not at the same level as the path, which introduces additional Y-offset amplifying the profile scaling. The resultant shape was unpredictable based on the algorithm.

Many thanks!