General Mechanical

General Mechanical

Thermal expansion of rigid connection

    • Mordrag
      Subscriber
      Is it possible to assign CTE to a connection based on remote points? For example, two bodies of the same material (same CTE) connected by a fixed joint representing the same material should under temperature difference loading show zero stress. However the introduction of rigid connection gives rise to the the artifical stresses where the remote points are attached. In nastran, one can define CTE for RBE2 connections which solves this problem, however Ansys handles these connections differently (I presume that Ansys doesn't have specific rigid body elements but connects the nodes by constraint equations CE).nRight now, I can think of only solving this by using beam connections, however by using this I get finite stiffness (if I don't use some artificialy high E for the beams which can lead to other problems..).n
    • Sean Harvey
      Ansys Employee
      ,nYes, so this had been an issue that was part of a feature suggestion and what you state is accurate. Let me see if I can find a solution. Thank you!nnRegards,nSeann
    • Sean Harvey
      Ansys Employee
      ,nSo, if you change the behavior on the remote point to beam, you can tailor the material radius and the material E to give you finite stiffness, and it won't need to be excessively high as rigid is really just an idealization. You can tailor as needed and unlikely you would need to make so high as to ill-condition the matrix, but maybe your situation is something I am not considering.nThe issue is that Mechanical is not applying the thermal load to the beam.nIf I take the setup from Mechanical into MAPDL, I can then use the bfe command with temp and specify the same thermal condition temperature on all the beam188s that got generated. When I run a model with this, I get negligible stress increases.nThe issue is to run this in Mechanical with out going to MAPDL, we will need some APDL commands to issue the bfe command to the beam elements that get generated. nAre you familiar with APDL? If so,then you can insert a command object, at the environment level, like you are inserting your thermal load.nIn that command object you can put in n/SOLUnesel,s,enam,,188nbfe,all,temp,1,100nallselnHere I am selecting all the beam188 that got generated and apply a temp of 100. You would need to elaborate this to limit the selection of beam188 (if you did not want to apply to all) or have other thermal conditions on beams on your model that this would interfere with. You also need to change the 100 to your thermal condition value (C,F,R, or K) careful with units.nI hope this helps.nRegards,nSeann
    • Mordrag
      Subscriber
      Thanks Sean ,nI have found a solution that fits me 100% in the meantime. I will describe it here in the case that someone would need it:n1.) Change to behaviour of remote point (RP) to beam, set the radius to 1 mm (exact value doesn't matter), set the beam material to a material with the desired CTE.n2.) Insert a command under each RP with the following (it will change the beams to MPC184 element which is rigid and with the given keyoptions it allows thermal expansion with the CTE from the beam's material:net,cid,184nkeyopt,cid,1,1nkeyopt,cid,2,1n3.) Insert another command under each RP with the following (it will store the beam element type number into a variable):nMY_RIGID_BEAM_1 = cidn4.) Insert command under the analysis (it will add a temperature BC set to ARG1 to each beam connection, the temperatures can be checked in APDL)nesel,s,type,,MY_RIGID_BEAM_1n*do,i,2,100ntesel,a,type,,MY_RIGID_BEAM_%i%n*enddonbfe,all,temp,,ARG1nallselnnThis process is quite tedious but it works. It can be easily checked by assigning the same CTE to all geometry and beam connections and setting the same temperature BC to everything then fixing 1 node a running the analysis should give zero stresses (under 1 MPa) and isometric deformation.
Viewing 3 reply threads
  • You must be logged in to reply to this topic.