Building models from imported surfaces

[MesaTactical]

This is a sort of general "how to proceed" question regarding building new models from already existing solid models.

We make parts for shotguns, so what we will typically do is send a shotgun platform out to a service bureau to get a 3D solid model of it back. Then we can use the solid model as a basis on which to build the new parts.

When the solid model is saved as a SolidWorks part, it appears in the feature tree as one or more imported surfaces.

The most straightforward way for a noob to start making a new part is to use the Convert Entities tool to sketch surface details and shapes to match the shotgun solid model. This works very well, and before you know it you have yourself a 3D solid model of a new part.

The problem is, the imported surfaces are still in the model. And you can't delete them, because the sketches from which you made your part need the imported surfaces as references (from using the Convert Entities tool).

What would be a better procedure for using the imported surfaces to make sketches to build solid features, one that didn't depend on the existence of the imported features in the model description?

In the illustration below, the tan model is the imported surface, and the green is the 3D solid model I'm building on the imported surface.

 

[TheTick]

If you're using SW2003 or later, you can use "Insert --> Feature --> Delete bodies". This allows you to delete solid and surface bodies when you are done with them.

"Delete bodies" appears as a feature in the feature manager. You can suppress, delete, or roll back before the delete bodies feature and your bodies return. Features referencing the bodies before they were deleted in the feature tree retain associativity.

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[MesaTactical]

Ah, I've done that before. I notice the bodies never actually go away, they just appear in the feature tree as deleted bodies. I suppose that is so that feature that reference the deleted bodies won't be knocked out?

 

[PlasticFantastic]

When I work with imported data or scanned curves, I generally model the part within an assembly. I create an assembly with the imported data as one componenst. Then create a separate part file within the assembly to create native geometry. In your situation you can use convert entities to create new sketches. This is cool because native geometry will update if there are changes in imported surfaces. If you dont wish to keep these relations , you can Right click on the part and List External references. Proceed to deleate relations as needed.

(Alternately in your case it looks like you might get some killer results with FeatureWorks which works great with prismatic surfaces)

 

[MesaTactical]

PlasticFantastic,

Thanks. Perhaps it's because I am still getting acquainted with SoldiWorks, but for some reason I experience difficulties sketching while in an assembly...

 

[engAlright]

SW2005 gives you the option when sketching to not create external references. So, you can put your "reference" part in an assembly, then create a new part and start sketching in the new part. Make sure the "Don't create exernal references" option is checked so when you convert entities no external references are created. You can then dimension, constrain or fix the sketch geometry as you need to.

Voila - your new part will then have no link to the model with the imported surfaces!

 

[MesaTactical]

Ah ha, here's the problem I had sketching in an assembly: for some reason, I can't figure out how to do an extruded boss. Under Feature Commands, all that I am offered is extruded or revolved cuts.

 

[MesaTactical]

Edit: Oh ho, I see what I need to do: start a new part within the assembly.

Holy cow, this might be the Holy Grail...

 

[engAlright]

Sounds like you're on to it - when you are editing the new part in place, just make sure that the "No external references" button is pressed. That will prevent Solidworks from creating external references, even when you relate sketches or features in your current model to the surface model.

One other thing - when you first insert your new part in to the assembly, DON'T drop it on to a face of the surface model instead drop it on to one of the principal planes (Front, Top, Right)

As you are going along, any features that have an external reference will be dispalyed with a -> beside them in the feature manager. If you don't have any of these, your new part has no relation to the surface model.

 

[DDunnJTC]

Mesa,

Not being able to extrude a boss probably means you're sketching in the assembly, and not int the part. In the assembly, right-click on the part you want to edit and select "edit<partname>". This is editing in-context. In the context of the assembly, that is.