Fillet Radius Problems, Inventor Professional 2021

[Anonymous]

I often have difficulty creating the correct radius fillets in my models.  I either get an error message indicating the geometry is too complex or Inventor will not create a large enough radius fillet.

In the Cleat model below, the fillet radius at the ends of the two horns should be 5/8".  The largest fillet radius inventor will create is 7/16"  Why?  This is a problem.  Like this cleat, I sometimes recreate models that were original created in Solidworks and Inventor doesn't seem to be capable of creating the same model.  Am I doing something wrong?  Is this a limitation of Inventor Professional 2021?  Need some help to sort through or work around this issue.

I can upload the .ipt file if that will help.  Let me know.

Thank you,

Cleat with Incorrect End Fillet Radius

[johnsonshiue]

Hi! The behavior does not sound right. For any geometry SWX can creates, Inventor should be able to. Otherwise, it looks like a bug to me. Please share the file here. Forum experts and I can help take a look.

Many thanks!

[Anonymous]

I've included the .ipt Inventor file. I hope you Autodesk can either determine what I have done wrong or have a work around. Like I mentioned, this occurs many times. Usually on these mooring Cleats and also on T-Head style mooring Bollards. Both are for the Maritime industry.

Thank you,
Mike Granata, PE

[evankok]

Not a solution.

Would the bottom vertical\height dimension for Loft\Sketch8 be too small to allow a full 5/8 fillet on the bottom of the ellipse loft?

What about the line (flat spot) that connects the .625 radiuses? Would that impact the starting point for the bottom fillet of the ellipse?

I would think that when adding the 5/8 fillet on the bottom of the ellipse it would want to cut into the rest of the body creating a failure.

I am guessing here.

Impressive Sketch1.

Solidworks creates the fillet with the same dimensions?

[JDMather]

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@Anonymous wrote:

Like this cleat, I sometimes recreate models that were original created in Solidworks and Inventor doesn't seem to be capable of creating the same model. 

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Can you Attach example *.sldprt file here?

From my perspective the modeling technique you are using is a disaster in Inventor or in SolidWorks.

I would expect to have issues using this technique.

I am not at all impressed with Sketch1.

[evankok]

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@JDMather wrote:

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I am not at all impressed with Sketch1.

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I am impressed with the time and effort it took to sketch it out and have it fully constrained on one sketch.

Would I  use it as a modelling technique? No.

[Anonymous]

Unfortunately I do not have the Solidworks CAD model.  Only a pdf version of the paper copy of the drawing.

I agree, sketch 1 is very complex and I didn't have the luxury of being formerly trained with Inventor.  First of all, I was using many more simple sketches to create these models.  And I still do with the more simple bollards and cleats.  With some bollards and cleats many simple sketches sometimes made it more difficult to later revise them or edit them to create additional sizes of the same family model.  So, I began creating sketches like you see in sketch 1.  Second, usually, I get incomplete old (as much as 70 years old) reference material to work from to recreate these models, missing dimensions and drawing views as in this case.  So I a need to create sketches of an entire view to generate the missing information.  Sketch 1 in this cleat is not as complex as sketches in some of the T-head bollard models.

[JDMather]

Use Equal (=) and Symmetry constraints - generally if you have duplicated a dimension, there is a better way.

If you want to compare Inventor and SolidWorks, I will compare Inventor and SolidWorks.

But I need solid evidence or it is not worth my time.

I might be able to find time to demonstrate how I would have done this model if you supplied the source information.

How/where did you get the dimensions that you used?

[Anonymous]

@JDMather , who are you?  I am not asking you or anybody for this comparison.  Please stop posting on this thread.  I will wait for a professional and not insulting response from an Autodesk employee.

[ampster40]

Good Luck with that.

You may have lost your one connection to successfully compare SW to Inventor files, reference JD's signature. 

Hope this all works out for you.

[kelly.young · Accepted solution]

Hello @Anonymous the geometry doesn't look like it can compute a 5/8" radius all the way around. A possible workaround is to create a Loft Tangent to a Point, see Screencast: 

Please select the Accept Solution button if a post solves your issue or answers your question.

[Anonymous]

Thanks, I tried a loft, but not tangent to a point at the end of the horn.

[johnsonshiue]

Hi! Here is another solution without having to compromise the Fillet3. Please take a look at attached part.

I did change Loft1 from Section Loft to Center Rail Loft (adding a straight 3D center line). After that, Fillet3 can go up 5/8" without a problem.

Many thanks!

[johnsonshiue]

Hi Mike,

Nobody is trying to insult anybody here. We are all trying to find a good solution to the problem. JD's comments about your modeling technique in this particular case may sound harsh. But, I do see some areas to improve. The issue with this model is unclean intersection. A lot of geometry was created without clearly defined intersection. Then you try to smooth the edges. This kind of model may run into problems down the road, particularly when you change upstream features.

I notice that you have very good modeling concept, since you create fillets and holes toward the end. This is the right approach. But, the base shape was not defined in a robust way. Let me take a look at the model closer and see if I can show you a simpler or cleaner approach. It is possible you have found the best approach already. But, I would like to see if there is room for improvement.

Many thanks!

[johnsonshiue]

Hi Mike,

I took a closer look at the model. Except the unclean intersection between the Loft and the Revolve, I don't see anything else worth changing. Attached is a slight variation of your original model. Please take a look.

Many thanks!

[lena.talkhina]

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@Anonymous wrote:

@JDMather , who are you?  I am not asking you or anybody for this comparison.  Please stop posting on this thread.  I will wait for a professional and not insulting response from an Autodesk employee.

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