Welcome to MCAD Central

Join our MCAD Central community forums, the largest resource for MCAD (Mechanical Computer-Aided Design) professionals, including files, forums, jobs, articles, calendar, and more.

Register Log in

Solid to Surface

nkpham

New member
Is there a way to convert a solid into a surface? I created a bunch of solids, but found out that they would be easier to deal with if they were surfaces.
 

nkpham

New member
does that convert the solid into a surface, or does it create a copy and the solid still exists?



btw, is it Feature>Create>Surface>New>Copy>Done

then, Sold Surf>Done?
 

lcoates68

New member
Surface copy does not convert the solid it only copies the surface of the solid. The new surface will reference the solid geometry so you cannot delete the solid without losing the surface. You can't convert a solid to a surface, you must create your surfaces.
 

gggggggggg

New member
try this:



export your solid part as an IGES file, then import the IGES back into Pro. You will have to adjust some settings, but you should be able to accomplish your mission.



Late
 

Brian_Adkins

Moderator
If you create two copies of the solid surfaces, you can then use one of them to cut away the entire solid, leaving the second surface copy behind... and everything will still be associative.



Not the best modeling practice, but it works if you are stuck...



-Brian
 

miked

New member
If you copy the surfaces, you shouldnt copy the entire surface of the solid as one feature.

It will be easier to manipulate if you have individual surfs.

Mike
 

adicar01

New member
yes lcoate68 had right,

but I mean In this way to keep your model in parametic shape.

Another way is to make another file (new part file) and use

the function

DATA Sharing -> ExtCopyGeom (external copy geometry), choose open (then open your original file), use CSYS for orientation (corelation between those two file) after that choose surfaces ref. -> define -> Solid surf (from previous model - to take all solid shape). ... or in this way you can copy another kind of geometry (edges, Datums, curves).

This function has a very powerfull option:

Dependent geometry - when you will stil have conection with previous file

and

Independent geometry - when you broke all relation with previous part.

All imported geometry is on surfeces. You can make this for take a part of your previous file or all the file.

... but !!! Yes it is a but

in this function is not available on Fundation basic module.

Please take a look if you have SHARED DATA enable (on Insert menu)

I hope this will help you.
 

Brian_Adkins

Moderator
Keep in mind that with all Data-Sharing features, there is currently no way to completely break the dependency relationship between the parent and child parts. Toggling the feature dependency to 'independent' prevents changes from automatically propagating through, but the parent-child relationship is still there... and systems such as Intralink will still track it.



The only way to truly disolve the parent-child relationship is to delete the data-sharing feature after replacing it with a 'dumb' or 'static' version of the same geometry (perhaps created through the IGES in-out process).



Just wanted to make sure you don't end up with Intralink ghost objects without knowing where they came from.



-Brian
 

nkpham

New member
yes... i'm still working with the bridge. the sweeps are still giving me trouble. it didn't before so i was wondering if i could just convert my original solids to surfaces instead of trying to resolve my problem. that way, i wouldn't have to create new solid sections to use the surface merge. i guess i'll just try to resolve the sweep problem then. thank you all for your suggestions.
 

nkpham

New member
I defined a 3d curve for my bridge and segmented it into smaller curves to tell me where the solid and hollow sections are. Before, I used these smaller curves in my sweeps, but they don't seem to work anymore. You suggested for me to trim the edges, but i'm not sure what you meant.
 

dougr

New member
I meant trim the corners, you may have miniscule intersecting (or non-intersecting as the case maybe) entities in you trajectory sketch..
 

Sponsor

Top