Hi,
In Solidworks I can emboss a sketch into a 'wavy' surface without difficulty.
If I try to do the same thing with Inventors 'Emboss' command It fails with "Only planar, cylindrical or conical faces are supported."
Surely there must be a way to acheive the same effect as in the first illustration, in Inventor ? Am I missing something obvious?
Solved! Go to Solution.
Solved by CCarreiras. Go to Solution.
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.
If this solved your issue please mark this posting "Accept as Solution".
Or if you like something that was said and it was helpful, Kudos are appreciated. Thanks!!!!
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
The CADWhisperer YouTube Channel
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 🙂
I thought your design intent was to wrap to face.
I guess I should have seen that as SolidWorks is limited to wrapping to cylinders or cones as well.
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Thanks Cadmanto 🙂
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)
You missed the step suggested of offseting the surface (body) to Extrude to.
Works the same in SolidWorks.
The CADWhisperer YouTube Channel
Thanks JD. 🙂
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
@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.
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Here is an example of Splitting a face of the part and then Thicken-Cut that face.
The CADWhisperer YouTube Channel
It looks like you have figures this out.
What I was talking about (and I used to do this in Solidworks as well) was a plane above the part. Not going through it.
Then with the offset surface which follows the same curvature as the outside surface wave, would give you your cut depth. I hope this makes sense.
If this solved your issue please mark this posting "Accept as Solution".
Or if you like something that was said and it was helpful, Kudos are appreciated. Thanks!!!!