22 Replies Latest reply on Jun 12, 2015 8:58 AM by Joe Galliera

    At least two bodies are interfering .

    Hani Rousta

      I am trying to mesh a assembly and I keep getting this error : at least two bodies are interfering .

      I checked the interference detections and fixed all the interfering items but still getting same error

      I tried with mesh control too

      Probably I am doing something wrong

      I am sharing the model here so you can have look at this and share your opinion

      I really appreciate your help


      Thank you

        • Re: At least two bodies are interfering .
          James Riddell

          You did the 'Interference Check' under the Evaluation tab and got nothing?  Is your assembly fully restrained?

          • Re: At least two bodies are interfering .
            kk cheng



            Simulation cannot accept these parameters thus the part or the entire assembly cannot be meshed.


            For example, the first fixed part of the assembly.

            1. There are 28 solidbodies in the part. Some are separated, some are interfering

            2. I tried combine them and it failed due to geometric condition

            3. I go to each feature (extrude) and check the merge result and some of them I got Zero thickness error.


            I recommend you relook to the part models and how were they created. Try mesh them at part level. If you fail on part, no need to say about assembly.

            • Re: At least two bodies are interfering .

              hello bruh . les potatoes du mcdo c'est un peu la vie donc voilà fais toi un burger et on en parle plus. i hope this will help

              • Re: At least two bodies are interfering .
                Joe Galliera

                Hi Hani,


                The multi-body Formwork Pier part has more than 100 interferences.  Save out the bodies to an assembly and you will be able to do an Interference check in Assembly mode. But...




                You're trying to solve the interference issue is like trying to see the forest from within the trees.  I would approach this model/problem from a different direction.


                Firstly, the aspect ratio of the model is at least 1000, so using Solid element mesh for everything will be time consuming to solve to be able to get any sort of accuracy in the results, and it will take a long computational time to solve if you ever do get it to mesh successfully.  It may not able be able to mesh or run based on the amount of RAM you have.  We've incorporated a Large Model Direct Sparse solver to try to alleviate the issue of running out of RAM for large problems, but in any approach with Solids it will take a very long time.  So any time that you save on simply using Solid elements will hurt you on the back end in solver time and also when you try to post-process results.  In the case here, or whenever you have a large aspect ratio, you should utilize structural element types, such as Shells and Beams.  This will require much more manual work upfront, but it will pay off in the end with solver time, results and accuracy!  (Some notes later on manual work to be done to prep model.)


                Secondly, even if the model isn't exactly symmetric, it is mostly Quarter symmetric and any assumptions that are made here in regards to the geometry could be worked out or dismissed in post-processing.  This alone will allow you to cut out a lot of elements.  To help you out with creating 1/4-symmetry, I would put your assembly into another assembly where you can more easily align it with the Global coordinate system.  This will make creating an Assembly feature for the symmetry so much easier.  If the assembly cut doesn't work just right, then you can go down into the individual parts to make them quarter symmetric (this is much more work, obviously), but the assembly cut with a open sketch should work.


                I would try to stick with compatible mesh as much as possible because again when analyzing the connections between parts that are bonded, it will be in general more accurate.  All this depends on how you were to prepare the model.  Where connections are less important to analyze, you can bond them using a manually-defined bonded contact set.


                In preparing the model for Shell elements, I go to the parts themselves and convert the solid bodies to surface bodies by using the surfacing tools, such as offset, mid-surface, extend, split, knit and more among others.  Where a compatible mesh is essential (where analyzing connections closely), you need to make the edge of the mating surfaces the same length so that the nodes align perfectly, here the split line tool from the Curves menu can help (you can search for the command if you don't know it).  Shells are also good when you want to analyze welded bodies because you can pick off forces and moments used in the weld size calculation, or simply bond surface bodies using the Edge Weld tool in Simulation.


                Are the tie rods really necessary to figure out the stress in them, or could you replace them with springs?  It's be a lot easier to define the pre-tensile load on a spring then for the tie rods.  For stress in tie rods, later you could simply find the force on the springs and then use F/A.  For tie rod nuts, you could do a small specific study on them.