## General Mechanical

#### Problem with choosing the surface for fixed support.

• bharathgl
Subscriber

Hello everyone,

I am trying to perform a simulation on a flange system with a metal gasket. When I apply a load of 30 KN on the bolts on each side (See attached image 1). Then, the tension chain will move down. When the tension chain moves down, the flank surface of the tension chain meets the flank of the flange and pushes both the flanges in an inward direction which compresses the gasket (See Fig 2). Hence, there is a force (60 KN acting on the flank of the flange from the chain). Now, I want to do a simulation only with the tension chain to check whether it can withstand the applied force without any deformation. While doing so I get different results when I fix (Fixed support) different surfaces of the tension chain. I am not sure about on which face I should use fixed support so that it represents the actual problem. Can someone tell me which face should I fix? e.g. The flank of the tension chain, drill hole.

Looking forward to your response.

Thanks in advance.

Bharath

• Dave Looman
Ansys Employee
Since the model is self-equilibrating you can fix any small surface that is out of the way of the load path. For example, you could fix the face shown below. Instead of fixing a face you could activate weak springs.nn
• bharathgl
Subscriber
nThanks for the response. There is a problem when I fix the face as you mentioned. When a load of 30 KN is applied through bolts. There is also a force of (approx. 40 KN) acting from the flank face the tension chain on flange see fig (flange and gasket is just to explain the case I am performing analysis only with the chain). The flank face of the tension chain rests on the flank of the flange. So, Shouldn't I need to fix that face? or Shouldn't I need to apply that load of 40 KN? nWhen I fix the face as you mentioned I got some stress and deformation results. nAt the same time when I fix only the flank face of the tension chain I get different results. nWhen I fix both the faces i.e. the face you mentioned and the flank of the tension chain I get different results.nIn this which is correct? Looking forward to your response.nThanks in advancennn
• peteroznewman
Subscriber
@bharathgl, nThe 1/8 model I suggested in your other discussion applies here too. That is a model that solves the complete assembly using symmetry.n

Hello everyone,I am trying to perform a simulation on a flange system with a metal gasket. When I apply a load of 30 KN on the bolts on each side (See attached image 1). Then, the tension chain will move down. When the tension chain moves down, the flank surface of the tension chain meets the flank of the flange and pushes both the flanges in an inward direction which compresses the gasket (See Fig 2). Hence, there is a force (60 KN acting on the flank of the flange from the chain). Now, I want to do a simulation only with the tension chain to check whether it can withstand the applied force without any deformation. While doing so I get different results when I fix (Fixed support) different surfaces of the tension chain. I am not sure about on which face I should use fixed support so that it represents the actual problem. Can someone tell me which face should I fix? e.g. The flank of the tension chain, drill hole.Looking forward to your response.Thanks in advance.Bharathhttps://us.v-cdn.net/6032193/uploads/0L2WJ9PG5VL7/1.pnghttps://us.v-cdn.net/6032193/uploads/P2COONC43MBN/2.pnghttps://us.v-cdn.net/6032193/uploads/RHDQURWHUBYI/3.pnghttps://forum.ansys.com/discussion/21454/problem-in-choosing-the-surface-for-fixed-support

• bharathgl
Subscriber
Hi peter,nOnce again thanks for the response. I will perform a simulation and I will update. nThanks a lot.nRegards,nBharathn
• bharathgl
Subscriber
Dear nI have performed a simulation but there is a stress concentration at the corner of the chain. I have used fillet and also tried with different mesh density and refinement. But still there is a stress concentration. Is this value true ? I dont think that this is a true stress value. Can you tell me how to deal with this ?nThanks a lot in advance.nBharathnn
• peteroznewman
Subscriber
nYes, this is a true value for an ideal linear elastic material, since you added a fillet and refined the mesh.nThe real material has a yield strength and will plastically deform when the stress exceeds the yield strength.nIn Engineering Data, click on the material for the chain and in the Toolbox on the left, open the Plasticity category. Drag and drop Bilinear Kinematic Hardening onto your material. This property has only two inputs, Yield Strength and Tangent Modulus. Input the Yield Strength, but pay close attention to the Units that are present when you enter your value. Change the units if you want before you type in your value. If you do not have the Stress-Strain curve for your material, you can use the conservative approach of assuming an Elastic Perfectly-Plastic material. Simply type a 0 for the Tangent Modulus.nNow in your simulation, the stress will not be larger than the Yield Strength. You can plot Equivalent Plastic Strain to see how much material around that fillet has plastically deformed.n
• bharathgl
Subscriber
Thanks ?@peteroznewman?. Your explanation is very useful. I have introduced bilinear kinematic curve and I entered yield strength as 210 Mpa. The strain value I got is 0.0012 mm. For such high stress (around 1421 Mpa). Will there be a strain of only 0.001 mm?.
• peteroznewman
Subscriber
nYou can only see a stress of 1421 MPa when using the linear elastic material. Once you introduce an Elastic-Perfectly-Plastic material, you will not see a stress larger than 210 MPa.nValues of strain are dimensionless. If you mean the strain was 0.0012 mm/mm that is a strain of 0.12%. This is entirely reasonable for a Total Equivalent Strain. There are three types of equivalent strain you can plot once you introduce plasticity: Elastic, Plastic and Total types. Total = Elastic + Plastic. If you are calculating a Factor of Safety, you would compare Total Equivalent Strain with the material property called Elongation at Break.n
• bharathgl
Subscriber
Thanks a lot for your inputs, . With your guidance, I have successfully performed the FEM simulation. See Figures 1 and 2. I have a small doubt in post-processing. I wanted to know how is the force distribution (F) at the knife-edge circumference see fig 3. For this, I have constructed a path along the knife-edge circumference see figure 4. Now I wanted to know how much force is acting on the gasket from the knife-edge tip along this path. I tried with probe force reaction but I cannot able to select that circumferential knife-edge. It will be very nice if you could help me further. I am looking forward to your reply. Thanks a lot once again. nnn
• peteroznewman
Subscriber
nCongratulations on a successful model.nIt is easy to plot the contact pressure, using the Contact Tool inserted into the Solution branch. The contact force needs more work. I can't give instructions on how to do that without first doing some research. Please Save As your model, and in that copy, delete the solution and the mesh and create an Archive file. You have to put that in a Zip file, then you can attach it to your reply. Say what version of ANSYS you are using.n
• bharathgl
Subscriber
nThank you so much for your response. I am attaching the FEM Model for your reference. Currently, I am using ANSYS R 19.2. I am trying to plot a graph like this see fig 5. The individual nodes can be combined within a millimeter cutting edge length and their forces are added to plot in N/mm. I am looking forward to your response.nnn
• bharathgl
Subscriber
?Kindly let me know if you have any problems while opening the file.nThank you. n
• peteroznewman
Subscriber
nI was able to open your model however I am limited to the Academic version for 19.2 and your mesh has over 80,0000 nodes, so I can't solve it. I might try to remesh the gasket to use fewer nodes and see if I can get the node count < 32,000. The gasket is sweepable. nThe part with the edge that presses on the gasket could be sweepable if you had repaired the body in SpaceClaim to remove the two extra edges.n
• bharathgl
Subscriber
Yes Sure. I found more elements were used when I sweep. That's why I didn't. The count can be reduced to less than 32000. I did an initial simulation with very less elements . Later, I refined the mesh to get accurate results. I have refined the mesh and now the count is less than 32000. Please find the attached model.nnThank you. n
• peteroznewman
Subscriber
Here is a mesh I like because it has nodes almost lining up at the contact point. n
• bharathgl
Subscriber
Yes I noticed penetration if there is no node at the contact point. But later I refined it. Could you please tell me how to plot that graph? Like, how to find the force or reaction force as I asked earlier?. I am looking forward to your response.n Thanks in advance.n
• peteroznewman
Subscriber
nUnder Analysis Settings, you need to turn on all the output quantities. By default, some of them are turned off to save disk space.nThen you should request a User Defined Result. This is the Element Nodal Force in the Z direction.nThat allows you to plot nodal force instead of pressure.n
• bharathgl
Subscriber
Thanks a lot. It worked. Thanks for sharing your knowledge.
Viewing 18 reply threads
• You must be logged in to reply to this topic.