Create part from object

[jcuppiii563]

Hi, what is the best way to make each of these ribs an individual part?

I want them to be individual parts so I can orientate them flat on my 3D printer bed.

This was created as a loft between two airfoils, then extrude feature was used to create the ribs. 

 

 

 

[CCarreiras]

Hi!

Depends on how skilled you are using Inventor.
The newbie way is to copy/paste the file, creating the same number of copies equal to the number of members you need.(i believe is 20)
Open each copied file, use "Delete face" tool, solid mode, and delete the solids you don't need for each specific file.

Then you have each file with the respective solid, after you delete the other ones.

Note:

If you need to change something again, the files will not update.
If you need that associativity between files and the master, you have to use other methods.

The process will be a little more complicated, but i can explain.

[kacper.suchomski]

I think it will be easier to duplicate these solids using a pattern:

1. Create a rectangular pattern
2. select the variant with the pattern of solids
3. select a new solid as the result of the operation
4. select your body in the graphics area
5. indicate any axis direction
6. enter 0 in the distance field
7. enter the number of solids in the quantity field

Expand the folder with solids and turn on visibility one at a time.
Then follow @CCarreiras  instructions to delete unnecessary spaces from each solid (different each time); this way you will get separate solids.

The last step will be to Make Components based on solids (Manage tab).

[CCarreiras]

Hi Kacper,

To go to the multisolid method, i would prefer to sketch some lines and use Split tool, solid moode, to split the members into solids. Then use the make components, or create Derive files.

I feel it's a more "clean" method than the pattern workaround.

...But, I don't know the level of knowledge @jcuppiii563  has, so i did not mention multisolids, derive parts, make components, etc, since these methods are kind of intermediate/advanced level.

[kacper.suchomski]

Cześć  @CCarreiras 

Recently, I've seen a lot of inquiries here about problems with Split, when the lines did not exactly intersect the body, so they were not sure and I did not propose this method.
As for the creation of components - agreed. This is intermediate; but it seems to me the right way, that's why the task and I believe that with our little help everyone can learn it.

An alternative is to copy individual enclosed spaces to surfaces and then stitch (or sculpt) these surfaces to new solids.
After which, of course, you will need to make components based on them.

[JDMather]

@jcuppiii563 

Can you Attach your file here?

[cadman777]

I would do it using Skeletal modeling:

1. Make your Wing Surface (or Solid).

2. Then set a WorkPlane where each rib will occur.

Note: One way to locate each rib is to make a Sketch with one straight line running the length of the wing and adding SketchPoints at each rib position.

3. Then attach a WorkPlane to each SketchPoint + Line.

4. Then make a 2d Sketch on each WorkPlane and ProjectCutEdges of the Wing to get a flat profile Sketch.

5. Then open a new SheetMetal Part file and Derive that Sketch part into it along with that one Sketch.

6. Then Extrude that profile.

Note: If you create a Parameter in the MasterSketch file for the thickness of these ribs, you can Derive that Parameter into the new SheetMetal part file and use it for the Thickness value. 

7. Save that part and then SaveAs that part to a new name (same but with a sequential suffix?).

8. Then open the new part file and Edit the Deriveed component and bring in the next profile Sketch.

9. Then Redefine the the Extrude to that Sketch (or if that doesn't work, delete the existing Extrude and make a new one).

10. Then repeat until all ribs are made.

11. Then open a new Assembly and place all part files at the WorldOrigin.

Done.