Learning Forum

[AliceMAlmeida]

Hello community! Please someone help me, it's urgent! I'm trying to solve a Transient Structural system, but when I start the command to solve, it stucks in the message "Creating Solve Input File". I've already tried:

• To uncheck the selection box of "Distributed" cores simulation;
• To check if the path name has a bad character (C:SimulacoesF56);
• To decrease the number of cores in the Solver Settings;

But nothing worked. I don't know what to do.

[peteroznewman]

Try changing the Number of Steps to 1.nInstead of having 1097 steps, use Tabular Data and have 1097 rows of data for the loads.n

[danielmartinezf]

Hey peteroznewmann

Try changing the Number of Steps to 1.Instead of having 1097 steps, use Tabular Data and have 1097 rows of data for the loads./forum/discussion/comment/92892#Comment_92892

I have a similar case, it's a static structural analysis and it keeps getting stuck at the same point: creating solver input file. I have 1 step and I'm working on a single PC, on a local drive. Another thread recommended working on local drives and you recommended lowering the steps to 1, which I did and that's why there are some suppressed loads in the picture:nnMaterials are set up correctly and bodies have their materials assigned. The mesh is up to date too, the fixed supports represent the pins that mount the represented wing to the fuselage and the connections are all bonded contacts. I don't know what else could be creating this issue.nEdit: I also performed the steps mentioned by the original thread creator. Also: in the Workbench the setup update will just fail, giving an error message along the lines of 'Update failed for the Setup component in Static Structural. The Setup component in Static Structural does not contain all entity types advertised in its component template, even after update'n

[peteroznewman]

Hey Daniel nPlease clear generated data on the mesh, save the project and save an archive .wbpz file and attach that to your reply so I can take a look tomorrow.n

[danielmartinezf]

Here it goes, thanks for the quick response.nn

[peteroznewman]

Hey Daniel nThe reason why this model stalls is because you have tried to mesh thin-walled solid geometry with solid elements. That is a mistake. Unfortunately, some of your thin walled parts have been united into a single solid such as this one.n You need to convert these solids to surfaces. You can do that using the Midsurface button in SpaceClaim. Or you can just copy/paste one side of the solid and discard the solid.nTry again when you have only surface bodies that you can assign a thickness property to the shell elements that the mesher will cover the surfaces with.n

[danielmartinezf]

Yes sir, it finally got past that stage after changing every body to a midsurface and removing duplicates/checking the model. Thanks for your helpn

[danielmartinezf]

ArrayWell, now after doing everything I'm getting a new error: There is at least 1 small equation solver pivot term (e.g., at the UZ degree of freedom of node 861148). Please check for an insufficiently constrained modelThe model now looks like this at every body/part/solid:n I supressed the contacts in order to get a solid body, and used share topology in SpaceClaim (I also thoroughly checked for duplicate midsurfaces that would lead to intersecting volumes). Fixed supports can be found at the lines that define the holes where the wing is attached to the fuselage at the root of the wing, and vertical loads are set at each rib to simulate the spanwise lift distribution. Here's the file too:nPS: Body sizing is used in order to eliminate the quad meshing failed on __ errornArrayn

[peteroznewman]

Hey Daniel nThe problem is that you have not connected all the parts together. Drop a Modal analysis on the model and drag and drop the four Fixed Supports down. You will find parts floating around.nNote that there are 6 zero frequency modes. Keep adding contacts until you get a nonzero first mode.n