Errors in the thermo-elastic Model Check with Beam Connections

Peter_MurPeter_Mur Member
edited October 1 in Structural Mechanics


I am performing a thermo-elastic analysis on a structure i.e. two parts (PCB and a Plate) connected by 4 bolts, which are modeled as beams (washer surface to contact surface). One FE modeling check I have to perform is apply a dT of 100 C, while making sure all parts have the same material CTE defined (i.e. 10 ppm), including my Beam188 elements, which I have done. Deformable Remote Displacement is defined on one of the surfaces as the boundary condition for the structural analysis. The stresses from this simulation must be very low under 1000 Pa to pass model suitabiliy check.

When 4 beams are defined I pass this suitability check, but as soon as I add any sort of contact which I will need in my future simulations for my thermal interfaces (Bonded,No Separation, Friction) between two parts, I get residual stresses up to 20-400 MPa near the beam connection area.

I have tried a lot of different combinations for the contact. The reason for using beams is that I need to extract axial and shear forces on the screws/bolts. Am I setting up something incorrectly?

Thank you in advance for your support!

Best Answer


  • Hmm, I think I posted this under wrong support tab.

  • peteroznewmanpeteroznewman Member
    edited October 3

    @Peter_Mur Model checkout using a constant value of CTE on all parts and a delta T is a well known technique for finding modeling mistakes in a linear model. As you said, when the fixed support is a single vertex, the solution should have "zero" strain (or stress) in the results in order to pass the check. It is only valid for a linear model. It is not appropriate to use this checkout if you have a nonlinear model such as Frictional Contact.

    You say you have some Bonded Contact in the model. While bonded contact is a linear element in the model, it can be used between two surfaces that have a gap (or overlap). Since you can't assign a CTE to the Contact elements, that gap causes a mismatch in thermal expansion across that gap. You can't have any gaps between surfaces if you want to pass this check. Go back to CAD and remove any gaps between faces that are to be bonded. If you do that editing in SpaceClaim, go to the Prepare tab and click on the Share button. That will enable Shared Topology. Then in Mechanical, the mesher will connect those bodies using shared nodes on the coincident faces and there will be no need for bonded contact. If you must use Bonded Contact, use Type = MPC and try to align the nodes on both sides of the contact.

  • Thank you very much for your response @peteroznewman !!! Your response raises a few more questions about using ANSYS. I don’t have access to SpaceClaim and I use Solidworks for all my modeling. I don’t think merging bodies would work for me, since I need to define different materials for different bodies to estimate properly the thermal stresses within my system, after going through this "suitability check". Here are two more questions on the topic:

    1)     How do I know that my thermo-elastic solution is correct then, if it cannot solve for thermally expanded bonded/no separation (linear) contacts? As an example, I made two identical blocks (50 x 50 x 3 mm) with the same diameter through hole (2.2 mm) in the center of the part, connected with the beam, all three made out of the same material. I tried MPC bonded/no-separation contact, which did not help to reduce the stresses to 0. Also, I am getting an increased amounts of stress as I decrease the element size, meaning I cannot trust this solution. Removing the bonded contact solves this issue, but it is not a realistic thermal model.  

    2)     How do I obtain stresses/loads on my screws/bolts from thermal effects? I need axial load and shear load variation at different temperature conditions on my system. Let’s say if two items are clamped by 1 bolt there will be a thermal contact between those two parts – so ideally, I have to model it as a frictional contact. Currently, this type of model does not pass the suitability check (as you said it is because the model is no longer linear). If I don’t model this contact then all my thermal load will “go through” the modeled beam, reducing my thermal flux through the system, making it an incorrect model.

    Thank you in advance!

  • peteroznewmanpeteroznewman Member
    edited October 4


    You misunderstand what Shared Topology is. It is not merging the solids like you would do in SolidWorks. It is a special feature of the ANSYS model prep tools: DesignModeler and SpaceClaim. It allows two bodies to exist with separate properties, but to have nodes shared at a coincident face. Do you have access to DesignModeler?

    You can get the same effect as Shared Topology, but with more work, if you ensure the coincident faces are imprinted on each other. What that means is if a small square face on body 1 is touching the center of a large face on body 2, you need to divide the large face of body 2 so that there is a small face at the center that perfectly matches the face of body 1. In Mechanical, you apply Mesh Controls on those two identical faces so the nodes are perfectly aligned. Then use Mesh Merge to merge the nodes on the coincident face. No Bonded Contact is required.

    1) Quick and easy model. In the example of two 3 mm thick plates with a 2.2 mm diameter hole at the center, choose a diameter around the hole, say 5 mm, that has zero thermal contact resistance. Imprint on each face of the touching surfaces a 5 mm diameter circle to get two annular faces on each body. Use mesh controls (Face Meshing and Edge Sizing) to get an identical mesh on each body, then use Mesh Merge. Or use Bonded Contact, type = MPC. Since the two faces have no gap, this will pass the zero thermal strain test. The bonded contact (or Mesh Merge) provides the constraint to allow a statics solution.

    The bonded contact or merged mesh inside the 5 mm circle is like the "no slip" region of a bolted joint. When you set each body to have a different CTE, there will be stress created by this bonded contact. When the CTE is identical, there will be no stress at this bonded contact because there is no gap.

    If you expect some heat will transfer between the rest of the 50x50mm faces, you can use No Separation or Frictional contact and specify a thermal contact resistance.

    2) Solid fastener model. In addition to imprinting a 5 mm circle on the faces that touch, imprint a 5 mm circle on the other side of the 3 mm thick plate for the washer/bolt head to make contact. Make a solid body fastener in the shape of a dumbbell, with a 5 mm diameter cylinder on each end of a 6 mm long 2.2 mm diameter shaft. Use bolt pretension on the shaft. Use bonded or frictional contact between the "head" cylinder and the 5 mm annular ring on the top plate and bonded or frictional contact between the "nut" cylinder and the bottom plate. At the interface between the plates where there was a Bonded Contact, change that to Frictional Contact. Since all these faces have zero gaps, this assembly will pass the Thermal constant CTE zero strain model checkout.

    The advantage of #2 is that heat can also be conducted through the fastener. Another advantage of #2 is that when the bodies take different CTE values, the frictional contact can slip if the expansion exceeds the limit of the frictional tangential force.

  • Thank you for the explanation and suggestions @peteroznewman ! Unfortunately, I do not have access to the Design Modeler license. I created a split surface model in Solidworks and followed your advice about creating face meshing, face sizing and node merging of the interface contact surface between two bodies. For some reason, I am still getting non-zero strain at this interface. The behavior of the model is exactly the same whether I use bonded MPC contact or node merge, as you pointed out. The stresses I get also don’t change with finer meshing (which is good) – so there is some other issue which prevents me from obtaining zero strain result. All materials/CTE are the same. Any thoughts?

    I haven’t tried modelling 3D screw yet, which I could try to do next, in this simple 2-plate example. Is there a way to extract Axial and Shear Forces in Newtons from the midpoint of the shaft on the bolt, like the information you get from the Beam Results? Ideally this is the way I would like to make my model - after passing the CTE model check. My main assembly has over 70 screws, so I was hoping that the BEAM element approach would make the assembly smaller and easier to setup.

    Thank you again for your support! 

  • peteroznewmanpeteroznewman Member
    edited October 4

    I expect you do not have a kinematic ground connection. This is required. An example of a kinematic connection for solid elements is called 3-2-1. One node has a Displacement BC set to 0 in X, Y and Z, this is 3 constraints. A second node, spaced in X from the first node has a Displacement BC set to 0 in Y and Z, leaving X free, this is 2 constraints. A third node, spaced in Z from the first two nodes has a Displacement BC set to 0 for Y, leaving X and Z free, this is 1 constraint. That makes exactly six constraints to prevent rigid body motion.

    For shell and beam models, it is easier because you just pick any node and hold all six DOF fixed. That doesn't work for solid elements because they don't have rotational DOF.

    The image below is the 100 C Thermal Condition with two Steel plates. I reduced the Force Convergence criterion to 0.001% from the default 0.5% to put a few more zeros in the maximum stress, but it was well below the 1000 Pa threshold you needed at the default setting.

    Change the bottom plate to copper and there is a significant stress at the bonded 6 mm diameter faces.

  • @peteroznewman Thank you again!

    I used Remote Displacement face, which I set as deformable, which gave me no stresses at my constraint face and only around the beam connection. Your 3-2-1 constraint suggestion did not resolve the stresses I have from the beam, and it shows the same result as with the Remote Displacement constraint. Unfortunately, I am using the ANSYS R19.1 and cannot open your version of the file, as it is v19.3 :( Is there a way for you to can save your example in the previous ANSYS version? Attached is the example I am working on right now.

    Kind Regards!

  • @peteroznewman So I ended up downloading the free version of ANSYS and opened your model/example. It does not contain the beam connection, which creates the trouble for me. After adding the beam to your model, the new version of ANSYS does give me a warning message " Thermal conditions will not be applied to beams created through remote connections or beam connections." Is this where my issue is coming from?

  • peteroznewmanpeteroznewman Member
    edited October 4


    Yes, remote displacement, behavior = deformable, can be used on one face as a kinematic connection to ground.

    What version of ANSYS did you save in that zip archive? It's not 19.1 because I have that installed and it can't open the file you attached. If you had mentioned you were using ANSYS 19.1, I would have created my example in that version. All I can do now is export the geometry to a neutral file and start over.

    I have a suggestion for you that I will show on yor attachment, I just need to know what version you downloaded, was it ANSYS 2020 R2?

  • I see what you mean about a Beam Connection and each end scoped to a ring face around the hole.

    I offered two types of connection, neither of which uses a beam connection.

    1) Quick and easy model has no beam and no bolt pretension. A bonded contact holds the parts together.

    2) Solid fastener model has no beam, because it has been replaced with a solid fastener. The solid shaft of the fastener can have a bolt pretension applied.

  • @peteroznewman I have access to ANSYS 2020 R2 student edition, but I mainly use ANSYS 2019 R1. Not sure why you are not able to open the 2019 R1 file I attached.

    Thank you for the confirmation that Beam Connection cannot be used for thermoelastic analysis - this is quite unfortunate, as it seems like I have to model all the bolts for my simulation. Seems like it is a very easy functionality which ANSYS is missing...

    For your two suggestions, I have some questions:

    1) If I just model the bonded contact, how would I extract Axial and Shear loads to estimate what the force is on this contact/this screw? I can't seem to find a way to access this information, which I can then use for my margin of safety analysis on the screws. In NX, a simplified approach can be used (RBE2+CBUSH+RBE2 , rigid elements + spring element) to get the load forces on the node where the screw shaft should be, without modelling the fastener. Is there a technique in ANSYS to get the same information?

    2) If I model solid fastener for all my screws, and then pass the CTE check - is there a way to extract Axial and Shear loads from the screws? I understand that I will get strain/stress on the whole bolt and this may be enough to get tensile stress margins. But I also need to perform gap and slippage analysis on the fastener, for which I require to know the forces it experiences. Just ran a quick simulation and it seems I cannot get a zero strain result with the bolt...

    Thank you again for your efforts and support!

  • @Peter_Mur Now I understand why I failed to open your archive with ANSYS 19.1. You wrote ANSYS R19.1 but what you meant was ANSYS 2019 R1.

    I tried a method that I hoped would work with a Beam connection, which is to use Remote Points with Beams out to the nodes on the ring face. Since these can be assigned a material, and the Beam between the remote points is assigned a material, I expected this to have zero strain under the 100 C thermal load, but it didn't, so I am disappointed.

    1) I am familiar with the NX/Nastran RBE2+CBUSH+RBE2 method of extracting fastener loads at holes. However, if you use RBE2 spiders over a hole, you must also assign a CTE to the RBE element to pass the thermal load check.

    I don't know how to extract the forces passing through a bonded contact. Maybe an ANSYS staff member will answer that question.

    2) If you apply a Preload to the solid fastener shaft, that is going to create a gap that will create a CTE discontinuity and may cause the stress check to fail. The solid fastener should pass the CTE check without a bolt pretension load. Attach your ANSYS 2019 R1 model archive in a zip file, and I can look at that.

    The 100 C load is a model check with special constraints to ground. After the model passes that check, you can apply different constraints and loads, such as bolt pretension, that would cause it to fail the test, but that is okay. It already passed, and now you are using the model to get useful results.

    If you implement a solid bolt fastener with frictional contact at all faces, you can use the Contact Tool to plot the Gap and the Pressure or Status. If the status is Sticking, then the joint has not slipped. There are also Contact Forces available on each contact. Read the ANSYS Help manual for more information.

  • @peteroznewman thank you very much for your help and confirmation about the beam connection!

    I modeled one screw with bonded threaded contact and frictional contact under the head. It passed the thermal check! I then applied 0.1 N preload as well and the stresses are the same for both steps (preload and dT=100), meaning that the check is also passed! Attached is my model ANSYS 19 R1. I will add 3 more screws to see if I get any errors!

    Yes, I will check the gap and frictional stress for my gapping and slippage analysis. As for the CFN/CFS commands, it does not seem to be in the list of user defined results I can extract post my simulation. Where do I enter "NLDIAG,CONT" function?

    Thank you!

  • Now that the analysis is non-linear it takes a lot more time to solve when I change material to Aluminum and FR4 for the plates, and the bolt out of SS304. Also, I am getting some errors when doing the same thing with the 4 bolt model:

    "The solver engine was unable to converge on a solution for the nonlinear problem as constrained. Please see the Troubleshooting section of the Help System for more information."

    Is there anyway to simplify the analysis setup? I will have a model with over 100 parts, where 70 of those will have to be screws.

    Thank you!

  • peteroznewmanpeteroznewman Member
    edited October 6

    Yes, nonlinear models (frictional contact) take a lot more time to solve, get used to it. Convergence problems are very common in nonlinear models. There are lots of discussions on "unable to converge" on this site.

    In your attached zip file, Bolt_Joint_Example_3D, there are some mistakes. The bolt pretension is wrong because it was applied to a body. The correct way to apply that is to one of the cylindrical faces between the head and the bonded end. Another mistake is Bonded Contact is still defined in the Contact 3 folder. That was required when there was no solid fastener. Now a fastener is present, you should change that to Frictional contact.

    Learn to use the Object Generator with Named Selections. You make one named selection of all the "Contact" faces and another named selection for all the "Target" faces. Each Named Selection can have 70 faces. You create one Frictional Contact, then use the Object Generator to make 69 more. Pay attention to how the Named Selection can automatically pick 70 faces by using the Same Size feature.

  • @Peter_Mur

    I have never used it, but there is an equivalent to the Nastran CBUSH, and that is the Ansys COMBI250 element. You can look it up in the Ansys Help system.

  • @peteroznewman Thank you very much for your support! I did try COMBI250 element from the joint, but it would not allow me to run the analysis. I ended up adding full 3D model of the bolts and matching the nodes between all my MPC bonded contact surfaces, through face sizing. This allowed me to pass Suitability check on my full model! It did take a lot of time to match all the contact surfaces in my CAD and make sure that there are no overlaps or gaps. Also, to analyze in more detail the forces on the Bolts, I added a 0N preload, to be able to perform Bolt Analysis and extract Axial forces on the bolts, although I do get the information I need from the Von Mises and Shear stresses on the bolt shaft portion. I also learned to use Object Generator - thanks for the tip!

    Perhaps Ansys can "fix" their beam elements to be able to perform thermo-elastic simulations in their next releases.

Sign In or Register to comment.