spiky mesh after calculation.

mmartin

Good afternoon to everyone:

Your help would be greatly appreciated. I am currently calculating a steel joint using 6 bolts.
I am performing a nonlinear analysis since I am using contact, tie bonds, and nonlinear material (steel).
As soon as the calculation was complete, some spiky elements appeared around the bolt holes
Do you know why this happens?
thank you

Manuel Martín, from Spain.

mmartin

I enclose the MW file just in case.

Sergio

Results looks ok, under Deformed View Settings adjust the Scale factor to 1 or some value less alarming. The overall displacement is less than 1mm

disla

Hi Manuel, Feliz año.

I would say there is some initial mesh penetration or too much clearance in the contact areas. If "Adjust" is active the nodes are projected strain free from slave to master. Those crazy nodes flying could be those adjusted nodes.

Moving direction gives you information about where they come from and where there is penetration or too much clearance.

As Sergio says doesn't seem too much but I think you could improve projecting the nodes to a cylinder shape on the holes area.

Victor

Looks like the reason those holes are faceted is "Fit midside nodes to geometry" is turned off for the two plates' meshing parameters.

mmartin

Good morning:

Thank you for your help I really appreciate it.

DISLA: I will remesh the bolts in order to improve the smoothness of the stem. Great 3d view of the bolt-hole connection.

SERGIO: Your are right. The displacement is under 1mm which is fine also for me.

VICTOR: I cannot activate "Fit midside nodes to geometry" because malformed elements appeared (negative jacobian). So, I had to disable this option(what a pitty). Do you know any workaround? I will change the mesher(I like to using gmsh, so I will switch to tetgen)
Thank you to eveyone.

Manuel

mmartin

You all are right.
I sort it out.
I turned "Fit midside nodes to geometry" ON.
I remeshed the stem of the bolts
and it works now!!!

Thank you very much(again).

Manuel

mmartin

I enclose you the deformed model.
Stresses decreased compared to the previous and broken model.

Thank you all .

Manuel

disla

Hi Manuel,

I would be very interested in validating or at least end up as close as possible to the Bearing capacity provided by EUROCODE 3.
I’m posting the EC3 result for this configuration.
I have changed the bolts to 8.8 as I don’t have 6.8.
I’m also posting the basic geometry as clean as possible I'm working with.

I would invite anyone interested to comment or provide suggestion to see if we can get as close as possible to the EC3 results with MECWAY/Calculix.

-Some point under consideration:

-Element type. (I’m using C3D8I)
-Stress Strain curves. (Bilinear with E/100 as tangent modulus)(* Victor)
-Mesh density for the different elements. (First trial 28.000 Elements)
-Pre-tension procedure (I’m using Fn= 70% * F u,b * Section Resistant )
-BC. (One end fixed , multiple contacts and Rigid body to apply load on the other end.)


(*) Note: Victor, I’m looking at the inp and I can see that the Bilinear Plasticity is written like:

*MATERIAL,NAME=S275_Beam
*ELASTIC,TYPE=ISOTROPIC
210000000000,0.3
*DENSITY
7850
*PLASTIC,HARDENING=ISOTROPIC
265000000,0
2100265000000,1000

I think that should be (2100Mpa+265Mpa)*1.000.000=2.365.000.000Pa

*PLASTIC,HARDENING=ISOTROPIC
265000000,0
2.365.000.000,1


Regards

disla

I think that should be (2100Mpa+265Mpa)*1.000.000=2.365.000.000Pa

*PLASTIC,HARDENING=ISOTROPIC
265000000,0
2.365.000.000,1

I see what happens. Seems like you take the second point of the line at a strain of 1.000 . Strain rarely should go beyond 0.3 (30%). As reference, EN code considers an allowable plastic strain of 0.05 (5%). I think using 1.000 could be causing some strange response.

Victor

Yea, it uses the impossibly high plastic strain of 1000 to ensure you never reach that because it's supposed to be an idealized infinite straight line. I don't think there are any problems with such a high value and CCX would linearly interpolate at the actual equivalent plastic strain between 0 and 1000.

mmartin

Disla, thank you very much for your model. Amazing.
I really like the way you use MW-groups and the new MW bolt pretension option which I am going to use from now.
I agree with you that we should go on investigating how to retreive moment-rotation plots of the joint. T I think we have to monitor some control point throughout time and plot the values previos some trigonometric calculations.
Anyway, I saw your DISLA-Bolt-model using frames; nice and smart.

And, good weekend to every one.

Manuel (mmartin)

disla

The hexagonal Bolt-model should be in fact be called JohnM-Bolt-model. Check the link below where it was first described. It's worth to spend a couple of hours and build a library.
Another thing I consider interesting to look at is the meshing. Look at the gmsh algorithm. I like to benefit from the high quality of it's surface mesh and then extrude. Beams are very suitable for doing that.

I have a lot of theory about connections checking procedures but none of them shows where/how to apply the loads. Force and moments usually come from a beam model and the node forces needs to be transfer to a finite 3D model. ¿How long should we consider the beam members to consider the submodel a good representation?
I can see you apply forces directly to the plate but that's not what is done in other software.

¿Does anyone knows or has some reference / guidance about this point?


https://mecway.com/forum/discussion/comment/5412/#Comment_5412