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embossing onto multiple surfaces

12 REPLIES 12
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Message 1 of 13
michaelkovacik
1991 Views, 12 Replies

embossing onto multiple surfaces

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

 

Mike K

12 REPLIES 12
Message 2 of 13
JDMather
in reply to: michaelkovacik

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.


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Message 3 of 13
michaelkovacik
in reply to: JDMather

See attached

Message 4 of 13
sam_m
in reply to: michaelkovacik

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).



Sam M.
Inventor and Showcase monkey

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Message 5 of 13
JDMather
in reply to: michaelkovacik

Something like this?

see attached

 

(I very seldom use Emboss)


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Message 6 of 13
michaelkovacik
in reply to: JDMather

Thanks

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.

 

Mike

 

PS

do you have a first name?

Message 7 of 13
JDMather
in reply to: michaelkovacik

Offset surface

Extrude TO surface

 

Jeff

Extrude To.PNG

 

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.


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Message 8 of 13
MikeKovacik4928
in reply to: JDMather

Jeff

 

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.

 

Mike

Message 9 of 13
sam_m
in reply to: MikeKovacik4928

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)



Sam M.
Inventor and Showcase monkey

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Message 10 of 13
sam_m
in reply to: MikeKovacik4928

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.extrusion1.jpg



Sam M.
Inventor and Showcase monkey

Please mark this response as "Accept as Solution" if it answers your question...
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Message 11 of 13
JDMather
in reply to: MikeKovacik4928


@MikeKovacik4928 wrote:

... 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.


It is not possible for one file to "corrupt" another file unless you use that file in another.
The file was created with an authentic student license of the software.

Simply examine the construction technique and then delete the file.

No harm, no foul!

 

The extrusion must be entirely capped by the offset surface you are extruding to, so offset all surfaces that are needed to cap. When you select the offset surface as the capping surface it will get all of them in the offset surface feature.


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Message 12 of 13
MikeKovacik4928
in reply to: JDMather

"Accept as solution"

Thanks

Opened the file, and have seen how you did it.

Have managed to reconstruct myself.

I see you have to be careful of which surfaces you offset or you get error messages.

I see when you select any one of the surfaces which have been offset, while doing the extrude, subtract, to

even though only one is highlighted it takes the whole lot.

 

If I save the file and keep it as an ipt without bringing it into any iam's or idw's, will I be safe and not get that education plot stamp? The way I understand it from the messages is that as long as I don't mix the model with any thing else (ie keep it separate) the watermark won't appear

 

Mike

 

 

Message 13 of 13
MikeKovacik4928
in reply to: sam_m

Thanks for your examples and explanations.

I see you used "quilt" on your one example, when I tried to change it to "faces" and selected all the same faces I got an error message.

Conversely on my example when I tried to used "quilt" it wouldn't work, only worked with "faces"

 

I will look at this command in further detail to see the difference between the two.

 

I see your use of "sculpt" in the other example, I will look at that command in further detail as well

 

Mike

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