Hello everyone. This is my first post so pardon me if this is a bit long.
I am conducting FE analysis on a plate 18m long and 7m wide (Due to symmetry I am just modelling 9m length). This plate has a plate (30mm wide x 100mm high) every 500mm as the deflection needs to be limited between supports. Supports are placed every second plate (1000mm apart) and a lug is placed in 3 places for each support plate where linear actuators will support this entire plate and will also deflect such that this plate assumes a shape of 90m radius arc. This is to be done to make a base for mould.
There are 6 load cases that I am conducting:
Case 1: Flat plate with self weight
Case 2: Flat plate with product weight (applied as pressure on area)
Case 3: Flat plate with product weight and moments added to simulate bending of walls that are built for product mould.
Case 4: Curved plate with self weight (Same as Case 1 but plate is curved)
Case 5: Same as Case 2 but plate is curved
Case 6: Same as Case 3 but plate is curved.
I am able to conduct FE analysis for Case 1, 2, 4 and 5 but when I am applying Moments on area after adding a Rigid Connection to a Reference Point and area on which moment is to be applied, this case is not solving for more than 10minutes on 6 cores.
I cannot attach files here as they are too big so I am sharing through my google drive.
And I should add that when I conducted a similar FEA analysis for a shorter plate (4m long x 7m wide) and applied moments the same way, It is computing results. What is wrong with Case6.pmx file?
After you downloaded it, copy ALL the data to your prepomax/Solver installation path, spooles should already be in there.
Now in prepomax all you have to change is the default solver to the ccx_MKL File:
@datsnl Indeed, Spooles can be really slow with large models.
Your model is essentially a thin-walled stiffened panel. Maybe you could simplify it a bit and use shell elements. It will be difficult to mesh this model properly with solids (especially with tetrahedrons) since you need at least 3 elements per thickness and that will result in an even larger mesh and longer solution times.
Thank you Philipp, this definately sped up calculation and it completed in 29s for me.
But when I check results, they are too, too high in terms of deflection and Von Mises Stresses.
Deflection on the plate at RP73 and RP71 are way beyond normal deflections compared to Case 4 which is the case where only -399mm -Y displacement is forced but the plate deflects around -512.8mm (in -Y) direction.
Stresses in the areas that were around 42MPa maximum, are beyond 146600 MPa for Case 6 where which makes no sense.
And loads on the supports which for Case 5 were maximum 8500N are now in 6 to 7 figures.
I wanted to update all on what are the results I am getting.
I created 1 single file and added all 6 load cases in it.
Strangely, first 3 load cases are showing comparable results to the individual cases I did earlier but Cases 4, 5 and 6 are showing loads on supports too high (as shown in image below).
Have you tried running these last three cases separately ? Also, which solver do you use now ? If it’s PaStiX then there’s a small chance that the results are incorrect due to bugs in the solver (there were some in the past).
I ran last three cases separately and the results are consistent with the previous AllLoadCases.pmx simulation.
I haven’t changed solver from Pardiso as mentioned by PhilippTheEngineer.
I did notice that the support is 75mm offset from where the outside edge of the turning force is applied which may be resulting in heavy loads. I am in the process of changing my model and will update if this makes any difference to the loads and stresses.
After I did modifications to the step file by moving support closer by 75mm as I said earlier, I ran the same file (Cases123.pmx), for case1, 2 and 3 and they are fine.
Then I saved this file as a separate file (Cases456.pmx) and tried to run case 4, 5 and 6 and I am getting strange results.
So I went back to Cases123.pmx file and then copied it as Cases456.pmx and ran it (with single load case and case 1 boundary conditions and loads) and results are fine, then I modified boundary conditions as per Case 4 and results are out of whack again. I duplicated this Case4 as Case1 and added boundary conditions of Case 1 and the results are out of whack for Case4 but are fine for Case1.
Screenshot for Case 4 (all supports have 0mm displacement in Y direction and have gravity load case). My question is, why is there a notch at the support? and why is material intersecting itself?
Working on it step by step. The reason why I was getting high stresses and high load is that I had a Rigid Body constraint on a considerable area on the top plate (as shown in red colour in screenshot below). There are three areas with Rigid Body constraint, two horizontal and 1 vertical.
Next when I added displacement boundary condition on support as shown in screenshot below, it was fighting against the rigid body and creating high stresses and high loads on supports.
That is the reason why the first Case 4 I ran, without the Rigid Body constraint in it, did not have any high stress and high load but when I started combining all 6 load cases together, I started seeing this problem. As the rigid body is for the entire model and not related to a specific case.
Now I am looking for a way to apply Moment on the parts without Rigid Body. I tried applying moment directly to the node set but results for Case 6 in which I apply moment are similar to Case 5. Which is obvious as torque on nodes will only twist the nodes and not generate global twist.
However, regardless of the type of constraint, you may encounter similar issues if BCs interfere with constraints. Thus, you may have to change the modeling approach and the way load is applied to the structure. Details depend on how it’s supposed to be loaded in real life.
I had a look at the link for RBE3 integration in PrePoMax and tried a few things from that post.
I can summarise that,
Coupling → Distributing makes that surface that linking happens stiff similar to Rigid constraint.
Distributing Coupling with Dcoup3D is the right way for RBE3 type of connection as it did not change the surface stiffness from what it was previously.
By using Distributing Coupling with Dcoup3D, all of my load cases worked properly and here is the screenshot of the loads on one of the supports.
Hi @datsnl ,
could you share the entries you changed in the keyword editor ?
I tried a lot and i dont get the DCOUP3D to work.
It always gives me this error :
Next is Element connection which looks like the figure below. In general add it as following:
Element type DCOUP3D with ELSET defined above and a new element number not previously used, connected to a node number that you will define in step 2 below
next a new node number, not previously used, with its new co-ordinates defined
next, Distributing Coupling with ELSET defined in step 1 and in second line use the NSet previously defined, for me I had defined nwLeft, nwRight, nwEnd.
Thank you very much for your help !
I finally found the issue.
As you see above i gave the DCOUP3D Element a very high Element Number (123456789) just to be sure that i am above any other number.
Turns out this is not smart because depending on the highest element number calculix assumes the need of RAM.
So changing the element number to a 4 digit number helped me.
I also found that it is not necessary to give the DCoup3D element set a material.
I can confirm that it just workes like a RBE 3 Element.
From Coupling Kinematic which stiffens up the surface Coupling_Kinematic_TensionSample.pmx (2.7 MB)
