Good Morning Inventor Users
Is there any way of embossing onto
1. Multiple faces
2. surfaces that are not flat, cylindrical or conical
I have tried using the “stitch surface” command but I can’t seem to get it to select .
The surface was created using the loft command, but I don’t know how to select it as a composite surface
When I am doing the emboss.
Maybe it has to be done using another method besides emboss? How?
Any help appreciated
You can only Wrap to cylindrical or conical faces.
Sometimes you need to make the sketch visible agian and apply several embosses - one on each face, but you cannot wrap.
Occasionally you can use Delete Face with Heal to combine two faces into one face.
Attach your file here.
It is hard to tell from your image what you are trying to do.
The Plastic Part - Grill tool might get you what you need even if your part isn't really plastic or the feature isn't really a grill.
There's a few ways to skin the cat:
If that mesh will extrude then it can be easier to offset the relevent outer faces as a surface and extrude the mesh to the offset surface (with the offset distance being the emboss distance) for a cut operation. For an add opperation you can extrude from the sketch to the part and then use split with the offset surface.
If the mesh is more complex and then extrude as a collection of surfaces and offset the outer faces (as before) and use the sculpt command to do the emboss (either add or subtract).
Something like this?
(I very seldom use Emboss)
But I can't open your drawing it gives me the following error message.
I am working on Inventor 2013.
Maybe you can just describe what you did, so I can try it out.
I am on my home now.
Will log on again from home.
do you have a first name?
Extrude TO surface
Didn't know whether you wanted to add or cut material.
Simply change offset surface direction and Extrude From-To (Between) the solid and surface if adding material.
okay I am at home now. I don't want to open your file, I see it was created on an educational version. I believe that files opened on educational versions corrupt authentic software with the dreaded educational stamp.
I have offset the surface. Now when I try do an extrude between the plane I created the sketch on and the offset sur
face I cannot select the offset surface. It won't select OffsetSrf1 in the browser, and if I try to select the offset surfaces in the model it is extremely difficult to see them, and only slelects one at a time.
I'm still on 2012 so can't open your model, but will try to explain...
change the view to show hidden lines, which might make selecting the internally offset surface easier.
if you offset the outer surface as a single quilt instead of offsetting each surface individually it should just be a case of selecting 1 face on the quilt (make sure it is going in the correct direction - might have to change the "alternative solution" in the More tab of the extrusion dialog box).
or extrude the profiles as surfaces and use sculpt to get the same result.
see the attached two examples (made in 2012)
no need to do the cut between the sketch plane and the offset surface, just do a "to" and then the surface.
also, notice your example picture - the cut direction arrow is pointing up, so suggests you might need to change the direction in the More tab, as I mentioned in the last post. Here's a picture - check if it works by changing the button here.
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