cancel
Showing results for 
Search instead for 
Did you mean: 

Close a solid body by new surfaces

Pioneer
Pioneer

Hello to all,

I am pretty new with NX surfacing but I would like to do what I explained on the image bellow.

Is there any way to close this solid by these surfaces or I have to use Sew option which works only with Sheet bodies?

img03.PNG

15 REPLIES

Re: Close a solid body by new surfaces

Pioneer
Pioneer

Here is what I actually want to do. I have used so many option to get the results and I would like to hear your opinion to reduce number of operations. Any suggestion is very appreciated.

Danijel

Re: Close a solid body by new surfaces

Honored Contributor
Honored Contributor

There are several ways to accomplish that; probably the easiest would be to use "delete face" to delete the internal faces and allow the existing top and bottom faces to close up the volume.

 

Edit: the reply above applies to your screenshots and not necessarily to the model in the zip file. I'm not really sure what you are trying to accomplish in the model, would "unite" do the trick?

Re: Close a solid body by new surfaces

Pioneer
Pioneer

cowski1 wrote:

There are several ways to accomplish that; probably the easiest would be to use "delete face" to delete the internal faces and allow the existing top and bottom faces to close up the volume.


I undesrtand what do you mean. By deleting the insternal faces solid will be converted to sheet.

Another problem that I am trying to solve is conncected with the surface that I am using for trim. Those surface is always different and curve that I am using to create surface is imported as .dwg. How to prevent breaking of the features which happen when I import another sketch? This problem I am trying to solve for a long time.img03.PNG

Re: Close a solid body by new surfaces

Genius
Genius
No, it will not necessarily convert the solid to a sheet body if you use Delete Face in the Synchronous Modeling feature group. Instead of adding features to your modeling history, why not revise your approach by removing or replacing the Thicken with an Extrude or another similar feature?

If you're always going to import geometry instead of create it, get used to the parents "breaking" (not updating correctly). If you look into Replace Feature, this can be a bit less painful but you will have to go through a remapping process for the new curves. Most of it will depend on the complexity of your incoming sketches and whether they will contain the same number of curves or not.
-Tim

Re: Close a solid body by new surfaces

Phenom
Phenom

Delete the internal face with the 'heal' option enabled.

Ciao

Re: Close a solid body by new surfaces

Honored Contributor
Honored Contributor

"By deleting the insternal faces solid will be converted to sheet."

Not necessarily; it depends on the options you use in the "delete face" command. If the existing faces can grow to enclose the volume, they will and a solid will result.

 

"Those surface is always different and curve that I am using to create surface is imported as .dwg. How to prevent breaking of the features which happen when I import another sketch? This problem I am trying to solve for a long time."

 

I assume that you are importing new curves, updating the extrude feature with the new curves and other features fail or give warnings because of the new geometry. Here's a strategy that I use in cases such as this:

  • create the extruded sheet body with the curves
  • extract a copy of the extruded body (use the "feature body" selection rule)
  • use the extracted body for any necessary trims, the original extrude should have only 1 child feature: the extracted body
  • when new curves are imported, edit the extrude to use the new curves; the extracted body will update correctly and the change will cascade through all of the trim features that depend on the extracted body. To help minimize update errors, make sure that when you update the extrude, the surface normal points in the same direction as the original. You may need to select the replacement curves in a different order (or from the other end) if the normal gets flipped.
  • if the new curves are drastically different from the originals, some features may fail (mostly tapers and blends), but the major trims should update correctly.

Re: Close a solid body by new surfaces

Siemens Phenom Siemens Phenom
Siemens Phenom

I'm in movie-mode today.  Here's a couple of methods but not suggesting you use them - just showing what's possible with the delete face and unsew commands:

(view in My Videos)

 

Regards, Ben

Re: Close a solid body by new surfaces

Pioneer
Pioneer

Hello @TimF,

I will explain:

why not revise your approach by removing or replacing the Thicken with an Extrude or another similar feature? - Did you mean extrued surface with an angle instead of thicken option on drafted surface?

 

If you're always going to import geometry instead of create it, get used to the parents "breaking" (not updating correctly). If you look into Replace Feature, this can be a bit less painful but you will have to go through a remapping process for the new curves. Most of it will depend on the complexity of your incoming sketches and whether they will contain the same number of curves or not. - I have tried to avoid importing a geometry because of problem breaking of the features, but I still have not found a better solution. There are different types of the profile which I import. Profile sometimes contains just arcs, sometimes 2 lines and the rest of the geometry are arcs..etc. Here are some different types of the geometry that I import:

1.PNG2.PNG3.PNG4.PNG

Any advice is very appreciated.

Danijel

Re: Close a solid body by new surfaces

Siemens Genius Siemens Genius
Siemens Genius

@danijelVR

With regards to your original request to provide a simpler method to define your shape, see the attached part. There's no need to extract faces or patch surface openings.

 

Regards,

Abe