Let us clarify the issue. To begin with, this is not a pretension issue at all—the PRETENSION is doing its job just fine (with the addition of the boundary layer—a known practice in ccx).
The results underneath the bolt head look to me like sharp 90-degree edges. As a common practice, I wouldn’t blindly trust the results of either software. These are always problematic contact conditions, and they are handled very differently between software packages. I would look at the stresses at least one element away from the edge to see if these values are similar and base my evaluation from there.
Keep in mind that for contact stiffness values, calculix defaults to something like 50X the elastic modulus of the 1st material in the deck, unless you manually change that. I’m not sure about the default value in Abaqus.
I’d first check contact pressure and contact area to see the difference, then start changing the penalty factor in linear pressure overclosure from a rather “soft” value to a harder one, until result stabilizes. A single value is set in CCX, however the penalty factor depends on the contacting bodies’ stiffnesses divided by the characteristic length(s) - units, F/L^3 - . So you have to compromise to get accurate results at the critical locations. Uniform element edge length at the contact region is best for convergence and contact accuracy but its size has to be consistent with the stress gradient in the region (that is to be sure you have convergence).
The max stress on my end appears to be 171.8 MPa… Pretty close to your abaqus result of 168.7 MPa.
I did make a few changes to the input deck to make it closer to the Abaqus one- changes:
Removed the , Automatic from the *static
Increased the inc at the step level
These should not create such a discrepancy, but that was the only change.
MODELLO_PRET_edits
************************************************************
CalculiX Version 2.21 i8, Copyright(C) 1998-2023 Guido Dhondt
CalculiX comes with ABSOLUTELY NO WARRANTY. This is free
software, and you are welcome to redistribute it under
certain conditions, see gpl.htm
************************************************************
You are using an executable made on Tue Oct 10 18:21:26 EDT 2023
The numbers below are estimated upper bounds
number of:
nodes: 1906635
elements: 1911802
one-dimensional elements: 0
two-dimensional elements: 0
integration points per element: 9
degrees of freedom per node: 3
layers per element: 1
distributed facial loads: 0
distributed volumetric loads: 0
concentrated loads: 1
single point constraints: 9396
multiple point constraints: 2434
terms in all multiple point constraints: 19446
tie constraints: 4
dependent nodes tied by cyclic constraints: 0
dependent nodes in pre-tension constraints: 608
sets: 61
terms in all sets: 68309
materials: 2
constants per material and temperature: 8
temperature points per material: 1
plastic data points per material: 0
orientations: 0
amplitudes: 2
data points in all amplitudes: 2
print requests: 1
transformations: 0
property cards: 0
*WARNING reading *FRICTION: stick slope
must be strictly positive
the following default will be used: 95000.0000000000
the user is advised to analyze the results
carefully and, if possible, to come up with
a experimentally based stick slope
*WARNING reading *FRICTION. Card image:
0.121
STEP 1
*INFO reading *STEP: nonlinear geometric
effects are turned on
Static analysis was selected
Newton-Raphson iterative procedure is active
Nonlinear geometric effects are taken into account
...
Job finished
________________________________________
Total CalculiX Time: 479.822937
________________________________________
I noticed that the difference that Ifound was linked to *surface behavior. Abaqus works with hard contact, while Calculix with
*SURFACE BEHAVIOR, PRESSURE-OVERCLOSURE=LINEAR
1.e7,10
How can I simulate in ccx the hard contact?
Thank you
If I use the same card *SURFACE BEHAVIOR, PRESSURE-OVERCLOSURE=LINEAR
1.e7,10, the results are similar in both softwares.
If I use a default *SURFACE BEHAVIOR, PRESSURE-OVERCLOSURE=HARD
in Abaqus, the results are quite different.
So which value I should use in ccx to reproduce the abaqus default?
If you want to be sure that contact settings are the same then you should avoid defaults (hard contact or default linear relationship) and specify custom contact stiffness in both models.
might be interesting to increase stiffness from 1e7 to 1e8, 1e9, 1e10 until you face convergence issues. The biggest value probably will be similar to abaqus hard. Interesting for everybody to gain feeling on the use of the contact parameters.
I’m not sure where the difference is coming from at your end; From the picture you posted before, the models seem to be different- maybe this is a reduced model or something. However, the key thing is that I am getting nearly the same values with linear or hard overclosures (see below). Stresses are 171.6 MPa for the *SURFACE BEHAVIOR, PRESSURE-OVERCLOSURE=HARD contact versus 171.8 MPa for the *SURFACE BEHAVIOR, PRESSURE-OVERCLOSURE=LINEAR 1.0E7,10
Both results are consistent. Hard contact simply translates to 0.95E7, so it makes sense that it would be a lower stress.
The results I got a pretty close to the 168.7 MPa from Abaqus.
I would ask you: What is Abaqus’ default value for contact stiffness? We know Calculix’s 50 * E.
And I would agree with @Calc_em , avoid defaults whenever possible to really compare apples-to-apples.
I did not run abaqus- I don’t have a copy for personal use. I only used the pictures you provided.
