I have a simple 110mm long cantilever beam, created in Onshape, and used the technique described here to split the upper and lower faces 10mm from the origin to allow the fixed constraint to be applied on those faces to simulate a clamping force. I also defined 2 additional data points at 40mm and 70mm from the origin (i.e. 30 & 60mm from the clamped edge) to measure the strain on the top surface.

I need to apply a weight of 1kg (Fz = -9.81N) at a point on the top surface 90mm from the clamp, or 100mm from the origin. But I can’t seem to find a combination of distance/face that works. I either get no moment, if I choose face_0 in red above, or, seemingly the wrong moment in that the strain messurements are off by 3 times if I chose face_1 as below. In both cases I get a warning message though the simulation runs and finishes ok. How can I specify this correctly, or do I need to create an artefact in Onshape to apply the force to? If I am doing it right, why are the strain results too low (should be around 1400u and 700u but I’m getting 554u and 224u).

Hi @irving,

could you share your project with us please? If you do not know how to do that see: How to share a project

Cheers,

Jousef

Hi Jousef,

I’ve invited you to the project, I don’t want to publish a public link to this.

regards,
Irving

HI @irving,

"I need to apply a weight of 1kg (Fz = -9.81N) at a point on the top surface 90mm from the clamp, or 100mm from the origin. But I can’t seem to find a combination of distance/face that works. I either get no moment, if I choose face_0 in red above, or, seemingly the wrong moment in that the strain messurements are off by 3 times if I chose face_1 as below. "

So if I understand correctly you are applying a remote force to the blue point on the far right in your image and mapping that force to either the small top surface or the large top surface. When you apply a remote force that force is tied to every node on the surface you are selecting. So, essentially you are creating a distributed load on the surface. You are not creating a point load on the surface and this would explain the small strains compared to a beam in pure bending.

To get what I think you are wanting, one approach is to go into Onshape and create a small surface centered at 90mm and then apply the load to that surface. You can do this using the Split command that you used previously. Just make a rectangle or circle a few mm by a few mm and that should work for you.

Another option is to cut your beam at 90mm, the extra length you have does not affect the bending of the beam. Then in Simscale you can either apply a force to the edge or the end face.

I hope this helps. Please let e know if you have any other questions.

Thanks,
Christopher

1 Like

Christopher,

Thanks for your reply. I had an inkling that’s what might have been happening. I’ve used both of your suggestions in the past and was going to fall back on the ‘cut to expose a face to load’ approach. However this is part of an engineering course and later sessions will need to have a point loading so I was hoping this advanced analysis would mode would cater for that.

Hi @irving,

we could also think about applying a Dirac impulse with all forces being zero along the x-axis but with a force and the corresponding magnitude at the point you mentioned.

The idea by @cjquijano to shorten the cantilever beam was also my first idea but this is not a long-term solution and works not for every model.

Will have a look at that later on.

Best,

Jousef

Thanks @jousefm

Dirac impulse seems a bit overkill, as this is a tutorial aimed at MSc students and needs to be reasonably intuitive also they compare the results of this with a physical experiment run by a colleague.

I’ve had a play with shortening the beam as per @cjquijano’s suggestion and even that gives poor correlation with reality.Applying a load to the end face and a coarse mesh (2 layers of tets in my 1.5mm thick beam) gave 569u instead of 1400u measured - about the same as a distributed load (if that is indeed what I was seeing - the similarity of the result doesn’t convince me of that).

Then I tried a moderate mesh with 3 layers, that gave 927u, better but still a long way out. Then I tried refined the mesh, adding 5 layers to a depth of a 1/4 of the beam thickness. Surprisingly that made no improvement on the result, indeed it was worse at 775u Refining further to 1/2 depth and 10 layers gets me 1109 which is better still, so its clear I need a really fine mesh to get near real-world accuracy. But now I’m up to 122k tets which from past experience with other tools is far more than I would have expected for this problem (also in this last run no data was generated for the second point). So I backtracked and tried a moderate mesh with 2nd order elements. Success : ! 1426 and 713 - well within the tolerance required.

For the load issue I’m going to create another face 1mm wide at 90mm to apply the load to as that neatly models the cord used to hang the weight on in the real world.

Hi again @irving,

that is true but that was like the “last resort” that came into my mind.

Your approach is very interesting but requires some benchmarking here and there. I am happy though that you figured it out It would be nice if you invite me so that I can have a look at the post-processing results.

Keep us up to date when you test your new geometry

Good luck and happy simulating!

Jousef

1 Like

Hi @irving,

I am glad its working for you now. Second order elements definitely the way to go… always… almost.

Christopher

1 Like

Yes, all working great now. For FEA I think 2nd order elements should be the default. With those a default coarse mesh gives the expected result. I used a thin (1mm) strip as the loading area on the top face with a direct force of -9.81N which neatly models the cord they hang the 1 kg weight on in the practical experiment.

Thanks for your help guys @jousefm @cjquijano

4 Likes