Edit Thicken/Offset feature failed

[tedxzy]

Hi everyone,

This sheetmetal model was working fine, until I decided to check it against the original AutoCAD drawing. Once I finish the "Side layout" sketch, the two thicken features had exclamation marks.

   Create Thicken/Offset feature failed
     00014118master.ipt: Errors occurred during update
       Thicken7: Could not build this Thicken
         The attempted operation did not produce a meaningful result. Try with different inputs.

Thicken feature is where I left "End of part"

If I tick "Automatic blending", it still works, but I want to create a new solid. Can you please have a look for me? Thank you.

[wilkhui]

Hi tedxzy,

Thanks for posting on the forum - I'm unsure of the operations that you're attempting since the history tree of the part file that you attached doesn't contain any Thicken features (screen capture below).

Can you provide any further details?

Thanks!

Indy

[tedxzy]

Hi Indy,

Thank you for your reply. I want to put thicken feature between "Bend radius fillet" and "Outlet circle front". I think it's the top big radius, triangle face and side radius face cause problem. That front point has 3 lines join together. I can not thicken that 3 faces.

In attached photo, it shows what I want to do, but system gives me that error message.

Please try it for me. Thank you.

[wilkhui]

Hi tedxzy,

I'm not sure what's stopping you from doing this as the operation you describe is successful for me. I've attached my attempt (see Thicken6 in attachment) but it's made in 2013 with Service Pack 1.1 and Update 1 for SP1.1 - am I correct in thinking you already have the update installed?

Just in case, here's the link;

Update 1 for SP1.1:

http://usa.autodesk.com/adsk/servlet/ps/dl/item?siteID=123112&id=20857064&linkID=9242019

Hope this helps!

Indy

[tedxzy]

Hi Indy,

Thank you for your reply.

Can you try thicken same faces without pick "Automatic Blending"? I am trying to convert thickened feature into sheetmetal.

By the way, is there another way to create sheetmetal for this discharge chute? Can I pick faces to create sheetmetal? I think you can do that in Solidworks, from my memory.

Thank you.

Ted Xu

[ic198]

Hi tedxzy

Inventor doesn't seem to like fillets leaching into curved surfaces, or curved surfaces that come in tangential to others- you've got both going on in your part. I've had similar problems to yours a lot and have found several different ways to get round the problem. I have called the different solid bodies fixes, but in reality they are bodges to overcome a bug in Inventor... and it is a bug, there's no reason why it shouldn't work.

The command the Thicken command really doesn't seem to like in your history tree is Bend Radius Fillet, so for the first two bodges I used the other side or the part

Bodge 1: Create a surface from the faces using a zero offset. Apply the fillet. Thicken into a seperate body

Bodge 2: Thicken the faces into a seperate bodyt. Apply the fillet afterwards- you'll need to apply different fillets to the inside and outside faces for sheet metal to work but this can be done with parameters

Bodge 3: Doesn't work in your case, but sometimes has for me in the past- thicken each of the faces as a seperate thicken command, adding subsequent thickens to the previous body. I've labelled this one Partial fix...

Hope this helps

ic198

[tedxzy]

Hi ic198,

Thank you for your reply. I agree with Inventor really doesnt like curved surfaces that come in tangential to others.

I cant get it to work for the top sheet. I hope this can be fixed in the future editions. Inventor should allow us to create sheetmetals by just selecting faces.

Thank you again,

Ted

[ngen33r]

This problem still exists and it needs to be fixed. It is a nightmare trying to make molded parts of uniform thickness with surfaces when fillets have to be added after the thicken. 

[TheCADWhisperer]

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@ngen33r wrote:

This problem ... 

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What problem?

Can you attach your *.ipt file here?

[ngen33r]

I cannot upload the actual part but when practicing I tried modeling a cordless drill that has the same issue. It will thicken outward but not in and it is due to one of the fillets.

[ngen33r]

It is actually a waste of time to try and figure this out. I will just redesign the part so that the thicken will be from the inside out.

[TheCADWhisperer]

Just bumping this one - forgot all about it since it was hijacked to an ancient thread.