Hello everyone.
I am new to PrePoMax and I’m trying to simulate a steel baseplate fixing to concrete block.
The baseplate is fixed in 4 holes (imitating anchors). The force is applied to the top of the profile, which is connected to the baseplate by a Tie constraint.
When I try to run analysis then it show me an error:
*ERROR in add_sm_st: coefficient should be 0
I’ve been looking on the forum for the solution. I have found out that this error occurs when overconstraint or underconstraint appears. But I still don’t know how to solve it anyway. I’ve tried to add or remove different constraints in different places, even with help of the Internet, but it still doesn’t work.
I’ve also ran a frequency analysis and it looks like there is no contact between the baseplate and the concrete block, but I have added it.
Could you please look at it and try to help?
I am sending Google Drive link with pmx file: Prepomax - Google Drive
Yes, you have quite a lot of overconstraints here. Rigid body constraints mixing with tie and contact. Bottom plate also has a boundary condition applied. CalculiX is vulnerable to this.
In this case, contact mixed with tie constraint seems to be the cause of the error. It works if you replace contact with a second tie constraint.
Thanks for your reply.
The problem is that the baseplate can’t be tied to concrete block. It should be fixed only in holes (by anchors) and affect on concrete just like on a screenshot here:
I’ve made a model before that works, but it took a little too long to calculate (about 80 seconds). It was made with 2D and 3D elements. I am sending it below. I am trying to optimize time needed to do the calculations. That’s why I have made the model you saw. Is there some other way to optimize my case? Or maybe some way to make my 2D model work with contact?
You will have to refine the mesh to obtain accurate results anyway (and likely also add the remaining nonlinearities, further increasing the solving time). Shell elements in CalculiX are internally expanded to one layer of solid elements so you could use solid parts with one layer of elements (hex / hex-dominated mesh) in the thickness direction as well. Avoid tetrahedrons when possible.
Merging the two parts that were previously tied might indeed be a good idea, this way you will have one constraint less, reducing the risk of overconstraints. You could try doing the same with the shell model.
You will notice a big difference excluding the areas in tension from the contact.
The big center area under the plate is not in contact. Remove it from the contact definition.
the modeling is look complex for me, it can be simplified by spring/gap representation for concrete block and anchorage (axial & shear). Some modeling guideline is available from Comité Euro-International du Béton to defines all the stiffness value and curve by approximation.
*edited
add example problem setup (simple elastic linear for all part and component)
Technically, with a few modifications your model works. It’s important to know that calculix can not handle shells + rigid body + contact in one model in most cases.
So if you need rigid bodies + contact, you have to use solid elements.
So in this case i removed all rigid bodies (fixed the holes at the edges and applied “surface traction” to the column).
for shell contact, you must select the master + slave surfaces from the “right” side:
Hi,
sorry for not being clear, my intention was not to show the best way to solve the problem. He asked what he has to change to make his model converge.
I added preload just to show a new user that it is possible (and how), and not to compare the results with previous solutions.
indeed, i’m only quick looking since discrepancy of results seems to occur due to different model. My proposed model is commonly used and accepted, it is just alternate for question below.
