I'm guessing you can't mesh this? That's not too suprising, given the number of tiny features. If you want to mesh the entire model, either supress tiny features or turn up the tolerance, which will allow the mesher to ignore them. I'd probably not mesh the entire model, though. This looks like a (pseudo) plane strain situation. Even though you can't take a 2d section, you can cut out all but the smallest repeating section and you should get the same answer. This will let you use much much smaller elements, which will increase your odds of success.
I'd probably do some combination of the three.
what errors are you getting?
assuming you're having trouble meshing, +1 for mike's response. needs to be simplified. shells, symmetry, 2d...something. or you're going to have to have a megapower computer to solve the problem.
Hi Mike and Jared,
Thank you both for your replies and suggestions, am rather new to Solidworks simulation and trying it out with trial and error process.
Yes, am having heaps of trouble trying to mesh the model and it would give an error at each and every extrude cut or boss.
Would try out the suggesstions pointed out.
Did a revamp of the model and strip it down to it's bare minimum.
Am able to mesh model and achieve simulation results.
My question here, would the strip down (after simplifying) simulation model produce the same results as the actual (before simplifying) model?
But since we can't mesh the actual model we wouldn't know?
Simulation Test Results
I don't know the answer, but my suspicion is that if you remove a bunch of holes and stiffening ribs you change the result in unpredictable ways. You have also probably eliminated most of the buckling modes.
I'm with mike here.
one potential solution, build a smaller version and test simplified vs full and see what the deflection differences are. that will help you understand what the potential for error is between the models.
it also looks like you're using solids. take a look at beams and shells, you might be able to get this problem down to a reasonable setup with them.
In your simpifications you need to try and approximate the stiffness. So stiffening ribs are not likely something you can ommit. The holes...maybe turn to slots or remove and add a stress riser of 3 if they are not near a boundary. What elements did you use? Shells? The analysis looks like it may require a non linear solution but it depends on the deflection - if it deflects more than about 1/2 the strucural depth then NL effects are emerging to a significant degree. Are the segments structurally connected? What does the response of one look like compared to you simplified version of one?
How much RAM do you have on your computer? Since you are interested in displacement, you might be able to get away with "Draft" elements for a first pass. Also, looks like you can use Symmetry down the long axis to cut the problem in half. Finally, be sure you're using the Curvature-Based Mesher, which can adapt itself to feature size... See if that will mesh using finer settings. No guarantee and I have to echo the other suggestions, but maybe these brute force tips will get you through this one and allow you to compare simplified to non-simpliieid.
Hi Brian, 6GB of ram. When simulation is running, roughly about 3.5GB of ram is used up.
Thank you for the insightful and interesting methods, gladly appreciate each and everyone of them.
Have made some changes to the model which produced some advancement from where I first left off.
Have remodel this part in 'sheet metal' module and the ribs/extrusion are made using a 'form tool'. In addition to that have added in a 2mm radius on each of the corners of the profile.
Any further comments will be much appreciated.
Have look below:
1) Added 2mm Radius on the coners
2) Able to mesh the model but far from perfect
3) Trying to simulate this part placed on supports that are 40mm from either end, used 'split line' to draw the 40mm and add in a roller/slider fixture. Problem we see here is the missing mesh in-between the fixtures from both ends.
4) Same issue as stated in number 3; missing mesh
alexander, have you checked your method works or doesn't work with other simpler models?
sheetmetal conversion to shell is for simple sheetmetal parts. if it doesn't work, switch it to solids, and then define the shell manually.
i think i've seen some issues with converting forming tools and also split lines. in those cases, i've always gone with manual shells.
Have not tried it with other models as yet.
But might give a go with ur next suggestion which is to use solid modelling then shell manually.
Once again have made another attempt on this with the suggestions all of you have given.
This time, have drawn up the model in 'Solid' then 'Shell' it in mid plane.
Assigning shell thickness in simulation and meshing this time round is a breeze incomparison to what was previously done with a solid or sheetmetal model.
All the errors that were pointed out previously doesn't exist anymore:
Looking at results:
The displacement calculated in simulation is a far cry from an actual test done.
Just wondering could I have missed out anything here or done something wrong?
alex, draft or high quality elements?
are you confident that the loads and restraints in simulation match up to what you did in your physical test? (assuming here that the components also match up)
before you answer those, you might want to do a couple of quick checks with hand calculations. if you estimate the stiffness of your beam, does a hand calculation match the deflection you get in the physical test? does simulation match under those same conditions?
Loads wise yes, am pretty confident match up with simulation. It was done with approximately 10Kg increments. Have only done a 10Kg load test on this simulation.
Calculation wise, have to look and dig into it, you have a point there.
The query would be the fixtures I have inplaced for this simulation, which will investigate further.
might be worth posting some pictures of your test setup and a description of your boundary conditions. that would help from a comparison perspective.
When you did your physical test, were both ends of the beam held tight in a fixture, or were they able to "float"? It looks like you have both ends fixed in your simulation, which would limit the amount of deflection as the material has to stretch in order to deflect down.
Hi Patrick and All,
Yes, you are right when you say that physical test was done without fixtures held tight on both ends. Bascially, test specimen was placed on supports on both ends.
Please see pictures below for steps taken in Solidworks to create simulation:
1) Halved model in shell
2) Added 'Split Line' for use of Roller/Slider fixture as supports on both ends
3) Selection of shell model in simulation to assign 1mm thickness in total
4) Edges selected for symmetry
5) Roller/Slider fixture on face where 'Split Line' was added in image 2
6) Translation fixture added on selected face, model can only move in Y axis
7) 10kg or 101N Force added in total on selected faces
8) Isometric view of Forces, Fixtures and Symmetry on model
9) Mesh settings used
10) Isometric view of simulation result
11) Side view of simulation result
"placed on supports on both ends"
would you agree that means that the contact between your part and the supports would be a line vs the flat that you have created with the split line?
and that also at that line contact the component can rotate/pivot on that line and that the component could slide?
if so, you might want to reevaluate that boundary condition. by setting a roller slider all that you've done is set the nodes on that face to zero in the normal direction. so it will slide but only on that face and only in that plane. it will also remain flat.
you might also want to think about what your z direction restraint is doing on the back face.
consider a similar analysis on your load. you might want to see what happens if you apply the displacement you want at the symmetry face and see what load it requires. do you think your load creates that wallow in the middle at the center? (red)
a couple suggestions on this model:
1. could it be be made quarter symetric?
2. i might be reading your screenshots wrong, but what about applying your x directino restraint at the symmetry plane?
Thank you for your suggestions given.
That has definitely helped me understand better in thinking where and what fixtures to use.
If I have understood you correctly:
1) Y Axis fixed on the "Supports"
2) On Symmetry Plane, X and Z Axis Restrained
P/S: Reading from other posts and from other sources on net, since we are using half model, the Force applied will also need to be halved.
Getting there. How did you choose the rotational restraints?
Is it deflecting the way it did in your physical test?
Tried re-evaluating the fixtures.
Fixtures on "Support", by looking at part physically placed on supports:
- Translate freely in the X and Z axis
- Restraint in the Y axis.
- Rotate freely in the Y axis
- Restraint in the Z axis.
Not so sure about the X axis. Looking at it, I don't think the part will be able to rotate freely in the X axis. But when I tried applying a restraint on the X axis for rotation, I get an error stating there isn't enough fixtures.
End up using these settings:
Although this time round, the results for displacement at 7.15mm seems more realistic and closer to the actual test done, the fixture for rotation on the X axis still puzzles me. Can only guess that if a restraint is applied to the rotation on the X axis, the part will not be able to produce a deflection and be fixed as a flat piece.
Any further critique will be appreciated.
the x rotation, i don't think you should need to restrain that but then you have no restraint in the X direction which might cause things to get upset. but i don't think that restraint will cause things to be "incorrect" either. i'd continue playing with different settings on a simpler model to see what you get.
on your symmetry plane, consider locking down a point in the x direction and seeing if it runs.
but it looks like you're getting pretty close.
You currently have your force evenly distributed across each beam. Is that how your physical test was set up, or did you have a single load in the center?
Yes, the physical test had the load "evenly distributed across". Not a point load test for sure.