General Mechanical

General Mechanical

Error: ‘ Invalid Goemetry” in ansys mechanical

    • Ravikishan
      Subscriber

      the modal analysis is running fine. I tried to run the saw tooth shock with 20000g for 11ms. When I try to run the solution(/click solve) it throws an error of "Invalid geometry", the solution start running for some time and terminates. Please help for solving this problem. 

      load definition is done using time steps. please define setup for above requirement.

    • peteroznewman
      Subscriber

      Please reply with an image of the mesh, especially zoom in on a thin section and show how many elements are across the thickness. You should have at least two elements across the thickness.

      Is the mesh setting to Keep or Drop Midside Nodes?  It is better to Keep Midside nodes.

    • Ravikishan
      Subscriber

      i have ensured that there parts thinner than 2mm have more than one element through the thickness.

      i believe the images attached are relevant for help.

      few parts have midside nodes dropped for these shared images below.

      mesh infomesh metricszoom image of the complete productdetails of internal parts that are critical and checked for >1 element through thickness

    • Ravikishan
      Subscriber

      please check the attached archive file. 

      Ansys 17

    • peteroznewman
      Subscriber

      Hi Ravi,

      I'm looking at your model now and had a few questions and comments.

      I don't know why you get an "Invalid Geometry" message. There is no error shown in Solve.out, but the simulation runs.

      Do you know about Modal Superposition (MSUP) solution method for linear analysis?
      That is shown below.

       I assume that you don't want MSUP because you want a full nonlinear solution.

      Why are some of the parts meshed with linear elements (midside nodes dropped)? 
      Better results are usually obtained from quadratic elements (midside nodes kept).
      Some of your parts seem to have only one element through the thickness, which can be a problem.

      In the Transient Structural, the End Time for analysis is the same as the end of the ramp on the acceleration. I would have expected that the sawtooth would have occurred and then there would be a much longer simulation time to observe the response in the system to that "shock", like 100 ms.

      Where did the 20,000 G level at 11 ms come from? That sounds way too high. This webpage talks about a 20 G shock level at 11 ms. If you convert 20 G to mm/s^2, you get close to 20,000 mm/s^2. Is that what you meant?

      If you want the shock to end and the response to be calculated beyond, you can't use the formula that you have used, but you can break it up into a 3 step simulation, Step 1 ramps acceleration up to 20 G in 11 ms, Step 2 ramps down to zero acceleration in 0.1 ms and Step 3 keeps zero acceleration till the end time of 100 ms.

      It is better to use these settings under Analysis Settings.

      I'm running the model with these changes now. It converges on the first increment, then I stopped it to attach the ANSYS 17.0 archive. I will let it run out to 100 ms and reply if anything interesting happens. It might have a problem at the beginning of step 2.

      Regards,
      Peter

    • Ravikishan
      Subscriber

      Hi Peter.

      Thank you.

      for the surprise of "invalid geometry" i am clue less. it pops an error as "invalid Geometry" for every click of solve, though all the geometry refinement is done. while i've checked solve.out even i find '0'error.

       

      for the 20000G, the input is requirement of the application we want to simulate.

      this particular input will project the part in 'Z'-direction, it has to be propelled linearly in direction-Z.

       

      i'm not aware of MSUP relevance with current case. i'll explore that. 

       

      Midside nodes are dropped to reduce the number of nodes and in turn reduce the solve time. 

      please share any knowledge source related to optimizing mesh and reduce solve time. 

       

       

      i'll try solving the archive at my end. 

    • peteroznewman
      Subscriber

      Hi Ravi,

      My doubt remains about ramping up to an acceleration of 20,000 G in 11 ms.

      Double integrate the 11 ms acceleration ramp; the device displacement is 3.95 meters!
      Do you have a 4 meter (13 foot) long sled? 
      What happens once you reach 20,000 G in 11 ms? What is the profile after that?
      The sled carrying the device is traveling at about 1000 m/s at that time. 
      With zero acceleration it will travel another 10 meters in next 10 ms.

      The device has a mass of 3.385 kg, so to create the 20,000 G acceleration requires a force of 664 kN or 149,300 lbf.
      I expect this is an explosive method (pyro) to create that much force on this device.

      You say you are using linear elements to keep the node count down. I recommend you take all the thin bodies like PCBs and cover plates and make them midsurface models in the geometry editor and mesh them with shell elements. They will have more accurate bending response and take fewer nodes than the solid elements currently in the model. 

      In the model I left you above, I mistakenly used the Y-axis for the acceleration instead of the Z-axis. I also only used 20 G for 11 ms. Below is the simulation result from that run, which took about 20 hours on a 4-core computer to compute out to 15 ms. I hid a few of the outer parts to show the body with the largest deformation. It looks like a part of the PCB is missing. When you add the extra piece back in, it might stiffen this up to the point where it doesn't penetrate the other body, especially when you switch from Y to Z axis acceleration.

    • peteroznewman
      Subscriber

      The solver fails after 1.7 ms having ramped up to 3,090 G on the way to 20,000 G at 11 ms.

    • Ravikishan
      Subscriber

      i've changed the midside node to kept. and trying for a complete solve of 100 ms, it is solving from saturday

    • Ravikishan
      Subscriber

      i have difficulty in understanding your reply (bold-underlined below) regarding the double integration, sled velocity, displacement on sled, force transferred on the object. can you share any references for understanding the above topics. also will MSUP solve faster than this non-linear solution for a simplified view of the problem under study.

      <<

      Do you know about Modal Superposition (MSUP) solution method for linear analysis? -  i referred it from ansys help that modal super position will yeild a better solution

      Double integrate the 11 ms acceleration ramp; the device displacement is 3.95 meters!
      Do you have a 4 meter (13 foot) long sled? 
      What happens once you reach 20,000 G in 11 ms? What is the profile after that?
      The sled carrying the device is traveling at about 1000 m/s at that time. 
      With zero acceleration it will travel another 10 meters in next 10 ms.

       

      The device has a mass of 3.385 kg, so to create the 20,000 G acceleration requires a force of 664 kN or 149,300 lbf.
      I expect this is an explosive method (pyro) to create that much force on this device.

      >>

       

    • peteroznewman
      Subscriber

      1) MSUP does not yield a better solution, it yields a solution in less time than a Full transient analysis if the model is completely linear.  If the model is not linear due to a nonlinear material, frictional contact or large deflections, then you will not be able to run a MSUP transient analysis, you will have to run a Full transient analysis.

      2) In your first post you said, "I tried to run the saw tooth shock with 20000g for 11ms." I just took a second look at the image you posted below that statement and I see it has 2.1582e+6 mm/s^2 of acceleration. If I convert the number in the image, that is equal to 220g  not 20,000g that you wrote.

      In either case, the equations of motion are simple. Below are the Mathcad formulas I used, first with the value you wrote.


      Second with the value from the image.


      After 11 ms, the acceleration is zero, so the velocity at 11 ms is the constant velocity from then on. If you want to know how far it travels in the next 10 ms, in the first case you multiply 0.010 * 1,000 m/s to get a 10 m distance traveled.

Viewing 10 reply threads
  • You must be logged in to reply to this topic.