Inventor General Discussion

Inventor General Discussion

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griff701
Posts: 5
Registered: ‎10-03-2013
Message 1 of 13 (359 Views)
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The Emboss command severly limited?

359 Views, 12 Replies
10-03-2013 08:21 AM

Hi,

 

In Solidworks I can emboss a sketch into a 'wavy' surface without difficulty.

 

03-10-2013 15-53-26.jpg

 

 

 

If I try to do the same thing with Inventors 'Emboss' command It fails with "Only planar, cylindrical or conical faces are supported."

 

03-10-2013 16-02-10.jpg

 

 

Surely there must be a way to acheive the same effect as in the first illustration, in Inventor ? Am I missing something obvious?

Hi!

 

Sure you can, disable the "wrap to face" option.

 

1.png

 

Note: "wrap to face" will only work with cylindrical or conical surfaces.

 

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ccarreiras
Posts: 934
Registered: ‎02-04-2010
Message 2 of 13 (352 Views)

Re: The Emboss command severly limited?

10-03-2013 08:39 AM in reply to: griff701

Hi!

 

Sure you can, disable the "wrap to face" option.

 

1.png

 

Note: "wrap to face" will only work with cylindrical or conical surfaces.

 

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Regards.
CarlosC

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Cadmanto
Posts: 3,325
Registered: ‎12-07-2011
Message 3 of 13 (351 Views)

Re: The Emboss command severly limited?

10-03-2013 08:39 AM in reply to: griff701

Welcome to the forum.

I have nevered used the "Emboss" , but it seems to me like you could create a surface offset from the wavey surface into the part.  Then creating your sketch on the plane hovering over the part project a cut feature down to that surface and this should accomplish what you are looking for.

 

check.PNGIf this solved your issue please mark this posting "Accept as Solution".

Or if you like something that was said and it was helpful, Kudoskudos.PNG are appreciated. Thanks!!!! :smileyvery-happy:

 

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Scott McFadden
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JDMather
Posts: 27,610
Registered: ‎04-20-2006
Message 4 of 13 (341 Views)

Re: The Emboss command severly limited?

10-03-2013 08:54 AM in reply to: griff701

A recent discussion on the SolidWorks forum

http://forum.solidworks.com/  (well I went searching for the thread and couldn't find it quickly, but in the last two weeks)

reveals that the SolidWorks tool lacks some very basic functionality too.

 

But that aside, and since this is the Inventor forum, there are two basic work-arounds.

1. (as suggested) Offset a surface and the Extrude Cut to the surface.

2. Split the Face and Thicken/Offset cut.

 

You might make some suggestions here (I would really like to be able to wrap to a sphere (in SolidWorks or Inventor).

 

http://forums.autodesk.com/t5/Inventor-IdeaStation/idb-p/v1232

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griff701
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Registered: ‎10-03-2013
Message 5 of 13 (316 Views)

Re: The Emboss command severly limited?

10-03-2013 09:33 AM in reply to: ccarreiras

Thank you Carlos, thats exactly what I was looking for  - I've spent two days trying to figure that out, and it never occured to me to not check 'wrap to face'.

 

Thanks again :smileyhappy:

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JDMather
Posts: 27,610
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Message 6 of 13 (313 Views)

Re: The Emboss command severly limited?

10-03-2013 09:37 AM in reply to: griff701

I thought your design intent was to wrap to face.  :smileymad:

I guess I should have seen that as SolidWorks is limited to wrapping to cylinders or cones as well.

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griff701
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Registered: ‎10-03-2013
Message 7 of 13 (312 Views)

Re: The Emboss command severly limited?

10-03-2013 09:39 AM in reply to: Cadmanto

Thanks Cadmanto :smileyhappy:

 

The offset plane with the sketch would be as it appears in the second illustration in the original post ?

 

Cutting down from this sketch doesn't give a uniform depth of cut into the solid. It cuts more into the high points, and less into the low ones - unless I'm missing an option to enable that sort of cut. (Very possible - I'm very new to Inventor)

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JDMather
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Message 8 of 13 (309 Views)

Re: The Emboss command severly limited?

10-03-2013 09:42 AM in reply to: griff701

You missed the step suggested of offseting the surface (body) to Extrude to.

 

Works the same in SolidWorks.

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griff701
Posts: 5
Registered: ‎10-03-2013
Message 9 of 13 (308 Views)

Re: The Emboss command severly limited?

10-03-2013 09:45 AM in reply to: JDMather

Thanks JD. :smileyhappy:

 

I wasn't meaning to imply one package was better in any way than another - its just that using SW seemed the easiest way to illustrate what I was trying to do.

 

Splitting the body and then offsetting a sketch is another idea that never occured to me, but seems like a great suggestion.

 

Thank you

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JDMather
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Message 10 of 13 (291 Views)

Re: The Emboss command severly limited?

10-03-2013 09:51 AM in reply to: griff701

griff701 wrote:

Splitting the body and then offsetting a sketch is another idea that never occured to me, but seems like a great suggestion.


Not "splitting the body", splitting the face.
Not "offsetting the sketch", Thicken/Offset-Cut the face (I have to check if SolidWorks will do this the same way).

 

Here is an Example of #1 in SolidWorks (works the same in Inventor).  I will try to find an Example #2 in both programs.

 

Offset Surface.png

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