How to extract surfaces from a solid part/assembly?

[hamzabuttX6GV8]

Hello everyone, I recently switched from CATIA V5 to inventor. I haven't really worked on inventor before. So any help would be appreciated. How to extract surfaces from the faces of solid part? For example, if I want to extract the highlighted surface from solid model, how can I do that? I tried to use Convert to Form but it sometimes works and gives the error when there's a complex face e.g. in this case convert to form gives error when I try to get surface of highlighted cone.

Similarly I tried to use patch but it didn't quite create the same surface as that of the face of solid body (cone).

In Catia, there's a tool "Join" in surface modelling. You just have to select the faces that you want to create surfaces and click join and you simply get the surfaces. Is there similar kind of tool in inventor?

[SharkDesign]

Various ways to do this depending on what you're trying to get out of it. 

You can try doing a patch on all the surfaces you want. Might not get the correct answer that way.

3D model > Surface > Patch

You can try the new 'unwrap' command that will give you a flattened geometry of it. 

If it's sheet metal you can take it into the sheet metal environment, add some 'rips' to it and then flatten it. 

This shows how to do it without the rips part. 

https://www.youtube.com/watch?v=dAXE1iYkf5Y

Or, you can copy the surfaces into another file and do what you want with them in there. 

This example shows solids being copied, but you can use it for surfaces too:

https://knowledge.autodesk.com/community/screencast/27c1c09d-ff2f-44c4-9764-8605a79037aa

[JDMather · Accepted solution]

What is your goal?

One simple technique is Offset surface distance zero.

Derived Component is another technique.

Copy Object...

So many techniques depending on your Design Intent...

Can you Attach your file here?

[hamzabuttX6GV8]

As you can see in the attached picture, there are many faces in a single body. I want to extract surfaces from single body, thicken them and create an assembly of different parts instead of a single part consisting of all the faces.

Thanks, got what I was looking for.

Can you please explain derived component though?

[hamzabuttX6GV8]

This is not what I'm looking for. I want to extract the surface from a single part which consists of many faces (please see the attached picture above)

[SharkDesign]

Unwrap and copy methods that I mentioned would do this for you.

[JDMather · Accepted solution]

@hamzabuttX6GV8 

There are two techniques to do this.

Technique 1.

Offset surface distance zero.  Edit: You can skip this step, simply Thicken as new Body.  The offset surface works well if you want to add a bit of clearance.

Then Thicken as New Body.

This will give you multiple bodies within a single part file.

Manage>Make Components to push out individual part files and the assembly file.

Technique 2.

Start a new Part file.

Manage>Derive and select the original part file.  Set to derive as Surface body.

Thicken the desired surface to solid.

Build your assembly.

Both of these techniques are fully parametric - if you make a change to the original all will update to reflect the change.

[hamzabuttX6GV8]

Thanks.

I suppose "copy to object" command will isolate the surface from original part so that changing the original part does not have any effect on the previously extracted surface.
Am I right?

[JDMather]

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@hamzabuttX6GV8 wrote:
Thanks.

I suppose "copy to object" command will isolate the surface from original part so that changing the original part does not have any effect on the previously extracted surface.
Am I right?

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No, that is associative too. (But any of these techniques can be made non-associative by Break Link (or Suppress Link if you might want to restore associativity in the future.))

I did not explain the Copy Object technique.

Technique 3.

Place the part into an assembly.

Place (or start) a blank part into the assembly (actually doesn't have to be a blank part).

Edit the new part in the context of the assembly.

Copy Object to copy face of original part as surface body into the second part.

Thicken.

So this technique builds the individual parts from your master within the context of the assembly.

(In the background all of these are using Derived, the only real difference is the first technique creates multi-body solids.) 

I added a strikethrough correction to one of my previous responses - I hope you saw it as it is important.

[hamzabuttX6GV8]

Got it.
Thank you so much for your time and help.

[Borsht]

So you had to edit the offset surface to 0.  But that's truly what I want to do.  I want to add a surface body feature to my part geometry which is existing as a group of solid body faces.  Is this possible in the part environment.

[johnsonshiue]

Hi! Yes, this is doable. Offset may not allow you to select faces from different solid bodies. But you can create multiple offset surfaces. Then stitch them into one quilt.

Many thanks!