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Surface extraction

Question asked by Jim Steinmeyer on Mar 2, 2010
Latest reply on Mar 4, 2010 by Jim Steinmeyer

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We have a couple of interns working on Rhino designing a control counsol for us. They have designed a control paddle that needs to be molded. I can import the iges file into SW and make a solid with no problems. The vendor would now like us to give them a surface model so they can split it and create the mold. I tried shelling the model but that was not what they wanted. Apparently he wants just a surface model and both he and I are unable to create one. -I have never worked with surfaces before, Just solids. SW help tells me how to use the Surface Extraction Property Manager....but I can't find it on my machine to attempt using it. I also am not sure that is the best method to use.

Can someone suggest how to create a surface model, either from importing the Rhino surface, or by extracting a surface from the SW solid model?

Thank you

Jim S

Charles Culp Mar 2, 2010 5:53 PM

Correct Answer

Is he using SolidWorks as well?

If he is using SolidWorks, and you are sending him a .sldprt file:

1. Select the Body in the Body Folder in the Feature Tree. Sometimes this is automatically set to hide. So go to Tools>Options>System Options>Feature Tree. There will be a list of options to either hide, show, or "automatic". Make sure the one called "Solid Bodies" is set to show.

Do not select the body any other way besides selecting it in the feature manager tree, inside the "Solid Bodies" folder.

2. Use the Insert>Surface>Offset Surface tool. This will offset all the surfaces of that body. Set the offset distance to zero.

3. This will create a second body, which is a surface body. Make sure to either "Delete Body" the solid, or just hide it (from the body folder in the Feature Manager Tree).

If he is NOT using Solidworks:

When you export the part file, (to IGES or STEP), you can follow these steps:

1. Go to File>Save As... select whatever format you are using to export. Then click on Options... in the lower right.

2. There should be options. browse through them to find the one that says either "solid body" or "surface body". They will be called different things for different types, so use your intuition.

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Steve Ostrovsky Mar 2, 2010 5:14 PM

I should probably know how to do this with just the surfacing tools and I'm sure someone will dive in with a better solution, but ....

Insert the part into an assembly, then save the assembly as a part file and use the Exterior Faces option to create a surface model.

Butchered it, but should get the job done.

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Charles Culp Mar 2, 2010 5:53 PM

Is he using SolidWorks as well?

If he is using SolidWorks, and you are sending him a .sldprt file:

Do not select the body any other way besides selecting it in the feature manager tree, inside the "Solid Bodies" folder.

2. Use the Insert>Surface>Offset Surface tool. This will offset all the surfaces of that body. Set the offset distance to zero.

3. This will create a second body, which is a surface body. Make sure to either "Delete Body" the solid, or just hide it (from the body folder in the Feature Manager Tree).

If he is NOT using Solidworks:

When you export the part file, (to IGES or STEP), you can follow these steps:

1. Go to File>Save As... select whatever format you are using to export. Then click on Options... in the lower right.

2. There should be options. browse through them to find the one that says either "solid body" or "surface body". They will be called different things for different types, so use your intuition.

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Jim Steinmeyer @ Charles Culp on Mar 3, 2010 9:24 AM

Thank you Charles, That was a very helpful and complete explination. Just what an old dummy like me needs!

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Steve Ostrovsky @ Charles Culp on Mar 3, 2010 9:45 AM

I knew there was a better way. Been stuck in assemblies for a while and had that on the brain.

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Kevin Drew Mar 3, 2010 2:21 PM

Just another idea

You can right click on a back face or say something non functional then delete a face.

It will no longer be a solid model only a surface.

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Jim Steinmeyer @ Kevin Drew on Mar 4, 2010 9:49 AM

I just tried deleting a face and was not given an option to do anything other than deleating the whole solid. I did pick a surface and shelled the solid but that wasn't what the vendor needed but the offsetting the surface did provide the desired effect. I would be interested in how to delete just a face though if there is a setting I need to change.

Thank you.

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Kevin Drew @ Jim Steinmeyer on Mar 4, 2010 9:55 AM

Try insert/face/delete.

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face delete.jpg104.8 KB

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Jim Steinmeyer Mar 4, 2010 9:54 AM

Ok Shot off my mouth before full investigation. I opened the right click drop down and found the option to delete a face. I had to select the rest of the inside surfaces to get them to delete as well, but it did work quire easily.

Thank you

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8 Replies

Steve Ostrovsky Mar 2, 2010 5:14 PM
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Correct Answer
I should probably know how to do this with just the surfacing tools and I'm sure someone will dive in with a better solution, but ....

Insert the part into an assembly, then save the assembly as a part file and use the Exterior Faces option to create a surface model.

Butchered it, but should get the job done.
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Charles Culp Mar 2, 2010 5:53 PM
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Correct Answer
Is he using SolidWorks as well?

If he is using SolidWorks, and you are sending him a .sldprt file:

1. Select the Body in the Body Folder in the Feature Tree. Sometimes this is automatically set to hide. So go to Tools>Options>System Options>Feature Tree. There will be a list of options to either hide, show, or "automatic". Make sure the one called "Solid Bodies" is set to show.

Do not select the body any other way besides selecting it in the feature manager tree, inside the "Solid Bodies" folder.

2. Use the Insert>Surface>Offset Surface tool. This will offset all the surfaces of that body. Set the offset distance to zero.

3. This will create a second body, which is a surface body. Make sure to either "Delete Body" the solid, or just hide it (from the body folder in the Feature Manager Tree).

If he is NOT using Solidworks:

When you export the part file, (to IGES or STEP), you can follow these steps:

1. Go to File>Save As... select whatever format you are using to export. Then click on Options... in the lower right.

2. There should be options. browse through them to find the one that says either "solid body" or "surface body". They will be called different things for different types, so use your intuition.
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- Jim Steinmeyer @ Charles Culp on Mar 3, 2010 9:24 AM
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  Thank you Charles, That was a very helpful and complete explination. Just what an old dummy like me needs!
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- Steve Ostrovsky @ Charles Culp on Mar 3, 2010 9:45 AM
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  I knew there was a better way. Been stuck in assemblies for a while and had that on the brain.
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Kevin Drew Mar 3, 2010 2:21 PM
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Correct Answer
Just another idea
You can right click on a back face or say something non functional then delete a face.
It will no longer be a solid model only a surface.
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- Jim Steinmeyer @ Kevin Drew on Mar 4, 2010 9:49 AM
  Mark Correct
  Correct Answer
  I just tried deleting a face and was not given an option to do anything other than deleating the whole solid. I did pick a surface and shelled the solid but that wasn't what the vendor needed but the offsetting the surface did provide the desired effect. I would be interested in how to delete just a face though if there is a setting I need to change.
  
  Thank you.
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  - Kevin Drew @ Jim Steinmeyer on Mar 4, 2010 9:55 AM
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    Try insert/face/delete.
    Attachments
    face delete.jpg104.8 KB
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Jim Steinmeyer Mar 4, 2010 9:54 AM
Mark Correct
Correct Answer
Ok Shot off my mouth before full investigation. I opened the right click drop down and found the option to delete a face. I had to select the rest of the inside surfaces to get them to delete as well, but it did work quire easily.
Thank you
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