When comparing two models, when and why is it appropriate to compare deflections vs. stresses? For example, I have created a model of a concrete arch with 24 beam elements to investigate geometric nonlinear effects on a structure. I've also created a more involved model with 860 solid, eight-noded isoparametric type elements. For geometric nonlinear effects would comparing the deflections of the simple model vs. complex be adequate as a check for convergence?
Tek-Tips is the largest IT community on the Internet today!
Members share and learn making Tek-Tips Forums the best source of peer-reviewed technical information on the Internet!
-
Congratulations cowski on being selected by the Eng-Tips community for having the most helpful posts in the forums last week. Way to Go!
Comparing models with different elem.
- Thread starter gpg1
- Start date
- Thread starter
- #3
Corus,
Sorry for the confusion, but that is what I was referring to. I would like to use the simple model for further analysis and created the model with many more DOF's to compare deflections using a simplified load case. The deflections were pretty close, but another engineer suggested I compare stresses and not deflections. Thank you for the response.
Sorry for the confusion, but that is what I was referring to. I would like to use the simple model for further analysis and created the model with many more DOF's to compare deflections using a simplified load case. The deflections were pretty close, but another engineer suggested I compare stresses and not deflections. Thank you for the response.
We know that,
1) stress field is related to strain field
2) strain field is the derivative of the displacement field
3) In FEA, displacement field is calculated first then strain and stress fields are computed from displacement field.
As the other engineer suggested to you, it makes much more sense to check the stress field. Because, in a bad model your stress field doesn't match well with your theoretical (accurate) stress field. In fact, most of the proposed elements in FEA papers (specially shell elements) do only a good job for displacement field, but only few of them are good for stress fields. I am not talking about commercial codes, I guess that they programmed only the good ones.
AAY
1) stress field is related to strain field
2) strain field is the derivative of the displacement field
3) In FEA, displacement field is calculated first then strain and stress fields are computed from displacement field.
As the other engineer suggested to you, it makes much more sense to check the stress field. Because, in a bad model your stress field doesn't match well with your theoretical (accurate) stress field. In fact, most of the proposed elements in FEA papers (specially shell elements) do only a good job for displacement field, but only few of them are good for stress fields. I am not talking about commercial codes, I guess that they programmed only the good ones.
AAY
As feajob implies, models can be reasonably accurate for displacements but can be less accurate for stresses. If you're going to use a simpler model to describe something then you'll lose a lot of the accuracy in stresses as you're making more assumptions about the structure. For example, going from a 3D model to a 2D plane strain or plane stress model is making assumptions about the stress distribution through the thickness. However, using a simpler model allows you to use a more refined mesh at details in the structure. These details you may not be able to model efficiently with a 3D model. The results from the simpler 2D model would be better than from a more complex 3D model in this case, providing you understood the assumptions you were making when simplifying the geometry.
corus
corus
gpg1,
I'm not sure what you need out of the FEM model. If stress is what you're investigating then surely you will need to find a way to prove that your simple model is good enough to predict the geometric nonlinear effect. Otherwise it won't be neccesarry to correlate stress if deflection is what you want.
The way that I would approach your problem is by having a simple mesh sensitivity analysis. That is, you prepare 2-3 different mesh finess of your model(which you have got two) and plot the normalised stress vs mesh finess graph. then, by selecting a tolerance level on the graph (say 5% error) you should be able to work out how many elements you need to use for your model to provide the accuracy that you're after.
I'm not sure what you need out of the FEM model. If stress is what you're investigating then surely you will need to find a way to prove that your simple model is good enough to predict the geometric nonlinear effect. Otherwise it won't be neccesarry to correlate stress if deflection is what you want.
The way that I would approach your problem is by having a simple mesh sensitivity analysis. That is, you prepare 2-3 different mesh finess of your model(which you have got two) and plot the normalised stress vs mesh finess graph. then, by selecting a tolerance level on the graph (say 5% error) you should be able to work out how many elements you need to use for your model to provide the accuracy that you're after.
- Thread starter
- #7
Everyone,
Thank you for the input. I eventually would like to get a load rating (capacity/loading) of the structure (including geometric nonlinear effects) and I'm using a software that in the past has been notorious for having bugs/not performing well. As a check (or comparison)I've performed the geometric nonlinear analysis using the elastic simple model along with spread sheets to calc loads for the updated load vector, applied them to the model, gotten new loads,etc.
My calcs converged after three iterations. However, I'm assuming the simple model is deflecting accurately and because my load vector calcs are based on deflections, I created the larger DOF model. The program nonlinear run of the simple model had less deflection than my calcs and I have yet to compare stresses.
Chyriso,
I'll look more into performing a mesh sensitivity analysis.
FYI, the software I'm using will not take into account material nolinear effects. If there is one thing you can count on it's that concrete has compressive strength and it will crack. I've accounted for material effects just using simple code provisions.
Any other information anyone has would be most appreciated.
Thank you for the input. I eventually would like to get a load rating (capacity/loading) of the structure (including geometric nonlinear effects) and I'm using a software that in the past has been notorious for having bugs/not performing well. As a check (or comparison)I've performed the geometric nonlinear analysis using the elastic simple model along with spread sheets to calc loads for the updated load vector, applied them to the model, gotten new loads,etc.
My calcs converged after three iterations. However, I'm assuming the simple model is deflecting accurately and because my load vector calcs are based on deflections, I created the larger DOF model. The program nonlinear run of the simple model had less deflection than my calcs and I have yet to compare stresses.
Chyriso,
I'll look more into performing a mesh sensitivity analysis.
FYI, the software I'm using will not take into account material nolinear effects. If there is one thing you can count on it's that concrete has compressive strength and it will crack. I've accounted for material effects just using simple code provisions.
Any other information anyone has would be most appreciated.
- Status
Similar threads
- Question
- Question
- Question