15 Replies Latest reply on Oct 30, 2013 3:01 PM by Matt Gortner

    Volume Filler

      I have an imported CAD model of a valve, in which the interior is highly detailed. I need to forward a copy of this model to another company, but this company does not want the valve with all of the detail inside. Is there a quick way to fill the entire interior volume of a model in SolidWorks? The attached pic shows just a portion of the volume that needs to be filled.
        • Volume Filler
          Troy Peterson
          Do a Saveas "Part" you will get several options on the end result, pick the one that suits your needs best.

          Sorry, I thought this was an assembly.
            • Volume Filler
              Charles Culp
              Seal off the ends (with extrusions). Once you have an enclosed cavity, you can use "combine bodies" tool to fill your void. The steps go something like this:

              1. Make of copy of the body using "Move/Copy Body"
              2. Enclose cavity (see above)
              3. Create an extrusion (a large cube) that covers the entire part, but DO NOT check "merge result".
              4. Use "combine bodies" tool, and choose subtractive. Subtract the valve from the large cube. This should leave you with two results. everything inside the valve, and everything outside the valve.

              You now have a body that is the interior of the valve. Just combine it again with the original body.
                • Volume Filler
                  Charles,

                  My model was imported from an iges file, so in the feature tree, the only feature is an "imported" feature. I tried using the "Move/Copy Body" command, and the command is looking for two or more bodies for the selection. Is there a workaround for this step?

                  Thanks,
                  Don
                    • Volume Filler
                      Charles Culp
                      Sure, here is another method that uses the same tools, but works backwards. I have attached an example.

                      1. Cap the Ends
                      2. Create the cube to enclose the part, keeping "Merge result" unchecked.
                      3. Use "combine bodies", choose subtractive, and select both the bodies. When it asks which body to keep, select "by selection", and choose the outer one.
                      4. Create another cube, again without "Merge result"
                      5. Now use combine bodies again, this time subtracting the 1st "cube" from the 2nd.

                      See attached. Scroll down the rollback bar step by step to see how I did it.
                        • Volume Filler
                          Charles,

                          You sample file makes perfect sense. I think my problem is with my cad model. When I try to select the model to subtract from the cube, I get an error that says I need to select a solid body feature. I guess SW does not see the imported feature as a solid body, so it won't let me use it in the selection.

                          I greatly appreciate any additional tricks to work around this issue. Is it possible to convert the imported feature into a solid body that SW can recognize?

                          Thanks,
                          Don
                      • Volume Filler
                        Thomas Nunn
                        This method was really helpful. Can you take it one step further into an assembly?
                        I am trying to build an assembly with a valve centered in a large pipe, but not touching the pipe. How can I fill the volume between the valve and pipe in an assembly when the valve and pipe are two separate parts?

                        Thanks,
                        Thomas
                          • Volume Filler
                            Charles Culp
                            Thomas,

                            I think you are going to have to go into a bit more detail of what you want. Do you want a 3rd part file, that fills between the pipe and the valve? Or do you want the whole thing saved as a part file, and all one solid body? Both can be achieved.

                            Or is it something else entirely?
                              • Volume Filler
                                Thomas Nunn
                                Thank you for getting back to me so soon,

                                I believe the first method you proposed is what I'm trying to do.
                                The concrete filler used to suspend the valve in the centre of the pipe should be a third, separate part from the valve and pipe, which would then be mated into the assembly to fill the void.
                                But it also needs to be created in the assembly because its demensions depend on the two separate parts.
                                There are also configurations of this assembly which will contain multiple valve at different locations in the pipe.

                                Below is a simlified example of the pipe and valve assembly; it is designed to have a fluid flow through the system, but only through the valve opening.

                                Thanks again for your help,
                                Thomas
                                  • Volume Filler
                                    Charles Culp
                                    Thomas,

                                    I have attached an example that I created with your file. What I did was used "Insert>Component>New Part..." in your assembly, and then selected the "front plane" of the assembly. This created an in-place mate for this new component part, which I named concrete.

                                    Then, while editing the part in-context (while still having the assembly file open), I used the "offset surface" tool with an offset of 0.000. You will notice that this changes the name of the tool to "copy surface", which is what you are doing. I then selected all of the faces that would be required for filling between the two parts. I made some assumptions, and then trimmed the surfaces, and used "filled surface" on the ends. I could then "knit" the surfaces, and used the "convert to solid" check-box to make it a solid body.

                                    Like I said, I made some assumptions, so you may have to re-trim and/or revise the boundaries of the concrete to fit what you actually want. Let me know if this makes sense, and if it's what you are looking for. The concrete should be fully associative with any changes made to the original two part files, as long as they are just dimensional changes. If you start deleting/adding features, you will have to re-create the concrete.
                          • Re: Volume Filler
                            Matt Gortner

                            Charles' method worked for me but a colleague just shared a quicker method when the model is symmetric. This is an old topic but I thought this might help future users.

                             

                            1. If your symmetic part is not already cut in half, do so now.

                            2. Delete the face joining the outside and inside. You now have 2 bodies, inside and outside.

                            3. Delete the inside body (or hide)

                            4. Create planar face on the symmetry plane using open loop of the outside body

                            5. Knit into a solid

                            6. Mirror