spiky mesh after calculation.

mmartinmmartin
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.

Comments

  • mmartinmmartin
    I enclose the MW file just in case.
  • SergioSergio
    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
  • disladisla
    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.



  • VictorVictor
    Looks like the reason those holes are faceted is "Fit midside nodes to geometry" is turned off for the two plates' meshing parameters.
  • mmartinmmartin
    edited January 2023
    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
  • mmartinmmartin

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

    Thank you all .

    Manuel
  • disladisla
    edited January 2023
    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
  • disladisla
    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.
  • VictorVictor
    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.
  • mmartinmmartin
    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)
  • disladisla
    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
  • FatmacFatmac
    Hi guys - I was trying to brush up on my bolted connections and went back thru this model as a worked example. I do like this approach used here. However, one question that came out of it, what is the consensus on how best to deal with the washer, beam face contact. My feeling was that it should be a unilateral contact as in all the other contacts in this example. It appear that John has suggested it be tied and that looks like how it was approached in this example. I guess if there is plenty of pretension in the bolts it may not have a large influence on the out come? However it feels right to allow one side of the bolt to peel off the plate face? In some case the out come is quite different -I have attached 2 pics with the 2 different contacts and in this situation the difference is not huge but still different enough to be significant. The first pic is with unilateral, the second with tie contact -in both pics the deformations is well exaggerated (x30) to try and show the difference.
    I also have another question about grouping contact surfaces, are there any likely issues if a group of master and slave surfaces are put in one contact definition- in the pic attached I have collected all the underside of the washers together (on both sides of the beam) and made a contact definition with both top and bottom faces. The alternative is to make up many defintions for each washer face contact (pretty time consuming but perhaps necessary in some occasions??)
  • VictorVictor
    Part of the difference between *TIE and unilateral may be the contact stiffness which is effectively infinite for *TIE and looks a bit low for elastic in your screenshot. I would compare bonded elastic to unilateral elastic to make it more apples-to-apples.

    Yes, you can have many surfaces in the same contact definition. Just be careful that the wrong ones don't connect together - for instance, a plate with master and slave on opposite sides and nothing else in the same contact definition nearby can connect the two sides of the same plate to each other.

    Are you aiming to model the case where the plates slip and the bolts are in shear, or where they only provide tension? That might determine whether the washer can be bonded to the plate or not.
  • FatmacFatmac
    thanks again Victor for u quick reply. I will look and compare unilateral vs bonded elastic contact and see what gives. In my, very likely, over simplistic take on it, I was focusing more on the difference being more in the ability of the unilateral contact allowing the surfaces to part in some places, especially if there is any significant deformation around the bolt. My interest was to get a better understanding of the way bolt pretension affects this type of connection. On that matter I have been playing with 2 methods of applying the pretension- one with 'pretension section' and the other with shrinking the bolt by cooling it. Both appear to do what I'm expecting but the first gives a warning about the MPC being determined by the initial modeled positions of the nodes, not their deformed positions. I guess if the deformations are relatively small this is not an issue - if they are large are there other alternatives for adding the pretension? The cooling approach appears to work but its fiddle to arrive at a target pretension.
  • VictorVictor
    Just a thought, but perhaps it's possible to model the bolt in it's relaxed shorter state, then let the contact pull it to fit? You might have to write the contact cards by hand or disable the ADJUST parameter on *CONTACT PAIR. As with cooling, you might need to iterate a bit to get the required initial tension.

  • FatmacFatmac
    thats an interesting approach -i'll give that a go - thanks for that
Sign In or Register to comment.

Howdy, Stranger!

It looks like you're new here. If you want to get involved, click one of these buttons!

Sign In Register