Deleting Faces of a Solid Model 2

[rgmidway]

I'm trying to find a way to model in solids, then delete the faces and use the Thicken function. I really do not like the results using the Shell function, and the ease of future modification when working with solids is greater than when working with surfaces, imo...not to mention some customers requiring solid modeling.

Am I stuck working with a poorly processed shell function?

Thanks guys.

rg

 

[jackk]

Could you attach a picture of the part you're trying to build?

I thought Shell worked pretty good, so I'd like to learn about it's weaknesses. I also don't understand why you want to delete a face inorder to Thicken it.

 

[rgmidway]

What I am finding with Catia's Shell function is that it seems to work by offsetting the surface you are keeping, and then cutting out the section of the part that you chose to remove (while never actually removing the surfaces within the offset distance). By not removing your modeled surfaces first, the shell can be left with surfaces that do not "flow" around transitions in the part, but leave sharp steps along your trim edge.

When using Thicken, the material is added at 90 degrees to the surface at any given spot and gives a nice, smooth trim edge around all transitions.

I don't want to delete the face I am thickening, I want to delete the faces surrounding the one I want to actually use.

Thanks for your interest in this btw.

rg

 

[cadddict]

Why not extract the face you require to thicken and then remove the initial solid?

 

[Azrael]

I'm also interested to see that model. I'm basicly only working with shell now and have distanced my self from the thicken feature to no edge control and heavy update cycles with surfaces.

 

[rgmidway]

Here is an example of what I'm trying to explain.

It's a decently simple u-channel bracket, but the changes in angle of the surface are what caused the problems with the shell in the filleted regions of the edge. The picture shown is modeled in GSD and Thickened. You can see the front trim edge has nice smooth transitions around the fillets that I just couldn't replicate with Shell without creating extra splitting surfaces.

I don't really want to extract and remove because I want to keep the history of the part for easier future design changes.

So getting back to my original question...I take it there is no way to just delete a face off a solid model?

 

[catiajim]

In order to avoid the knife edges as you mentioned, we usually recommend that our users define these types of parts using GSD Surfaces, and then use the Part Design Thick Surface to generate the solid. We recommend modeling all of our sheetmetal parts that way (that is, until we get Aerospace Sheetmetal Design into production).

 

[itsmyjob]

rgmidway no there is no way of just deleting one face off a solid to make a solid like you need.

The GSD / Thick surface is (like Jim said) the best way of doing what you need.

The Shell is nice because you work in PartDesign and do not need surfacing training, but is not very usefull for 'sheetmetal' part.

The remove face function in Part Design is usefull when working on solid with no history...

i.e. Make a pad, then a hole. Copy/Past as result in a new file, then use the remove face on the face of the hole. Hole is gone. Works also on fillets, chamfer...
We use that in solid preparation prior meshing.

Eric N.
indocti discant et ament meminisse periti ​

 

[Azrael]

rgmidway

I would create the splitting surface but that's me. It's a simple part so I wonder if even I wouldn't create it with thick surf. An alternative way that I have used when shelling parts is that you create your part with surfs without any fillets apply a thick surf way bigger then wanted thickness, apply solid fillets and then shell it.

I have used shell on both BiW and Interior trim parts mainly because that I have control of the edges. In you case you have a triangular tilted faces that will have an edge pointing inward the part, is that the case when it's produces? But the biggest benefit with solid based modelling is updating specially when using multiple bodies where the bodies represents different geometrical featues.

Like caddict suggested you could use extract with propagation set to tangency and you will get all wanted surfaces in one shot, just remove the holes add them on the thickened surf

 

[rgmidway]

Much thanks to everyone for their input. I guess if the customer wants accurate Catia models, they have to settle for surface-based modeling. It's a shame though, feature bodies (like Az said) make updating so easy.

And yes Az, the edge pointing inward is the whole cause of this issue, but that is how the part is produced.

 

[kbro151]

I was able to make something very similar to the pic you posted using only pad, chamfer, fillet, and shell. How do I post a picture of it? I'm interested to know what teh exact sticking point is. I've run into problems with shell before too.

 

[rgmidway]

The red lines indicate 90 degree lines. The yellow is where the material flow transitions between each 90 degree. This yellow region is where you get knife edges using the Shell funcion.


And to post a picture, you can use

http://www.imageshack.us/

to host it and link it as specified in the notes you see on the "Preview Post" page.