Nonlinear Static Simulation of an Oil and Gas Multicontact Seal Application

ARNE KJAER: So welcome, everybody, to our presentation. The class in ENR501474, Nonlinear Static Simulation of an Oil and Gas Multicontact Seal Application. My name is Arne Kjaer. I'm the CEO and owner of PTFE Engineering.

I'm a polymer specialist and mechanical engineer from the Technical University of Denmark. I have 39 years of experience in development of material compositions and processing within the PTFE industry.

First FEA material model work was in 1992 with the University of Stuttgart. Polymeric material modeling for six years with Autodesk, Nastran, LS Dyna, COMSOL, and ANSYS. Met David first time at AU 2015 in Las Vegas.

David Weinberg, my co-speaker today, is a distinguished research scientist with Autodesk. David works for Autodesk Product Development and Manufacturing Solutions, Nastran Simulation and Generative Design group.

The primary developer of Autodesk Nastran and Inventor Nastran currently leads the team of developers of Autodesk Nastran. Over 35 years' experience in FEA simulation, working both as a user for several large Aerospace companies and as a developer.

David is also a retired US Air Force aircraft commander and pilot.

Together David and me, we have been doing two presentations before at AU. First time, AU 2018 Las Vegas where we presented Challenges of Simulating Advanced Materials in Nonlinear Applications. And then again in 2019, also in Las Vegas, with the title of Simulating with Nonlinear Materials like Hyperelastic and Isotropic Polymer Materials.

We have this safe harbor statement which is supplied to all people coming from Autodesk. This is a long one, we will just pass. Go on.

Today we will have some learning objectives. And this is prepare the inventor assembly to the Nastran Simulation. We will make setup of a nonlinear static Nastran analysis from in inventor assembly.

We'll try to use material model data from customer material measurements. Using multiple subcases using same constraints and loads. Setup of enforced motions and surface pressure. Optimize the mesh and mesh control to get reliable results in less time. And special parameters setting to help the analysis running.

And then we will have a look at the results, how to interpret those.

Today's case story is an inspection hatch in a machinery with high pressure and elevated temperature. It needs to be sealed off so the inside substance cannot escape to the outside. This hatch is constructed to be used for this demonstration of inventor Nastran 2023. This case is constructed only for the AU 2022 in New Orleans, United States of America.

Here we have a cross section of the hatch. And the hatch, you can see, have a upper lid here with some glass. And we have the machinery assembly where we have the sealing groove. And we have a seal sitting here with some support ring and some metallic springs.

We have in this case, we will be calculating with a pressure of 1450 PSI. And we will be calculating today the temperature at 73 Fahrenheit.

This is a little closer look to the assembly. And here we have the PTFE seal. And we have the metal spring and we have the so-called PEEK backup ring. The PEEK ring is preventing the seal from extruding into the gap here.

The case story is that we need to make an assembly to be able to simulate it. The metal spring has to be exchanged by a spring force or a surface pressure. So this spring here, we will need to get the spring out of the assembly otherwise before we can simulate it.

And what do we simulate in this class here? We simulate that we have the groove, the metal groove, here. We have the lead, we have the seal. We have the PEEK backup ring. So what we are doing is we are applying it in fast motion to the lid. So closing down the lid so the seal gets activated.

And then inside the seal, we apply a spring force. And then we apply also hydraulic pressure inside. And this is the result when we have the high pressure and we have the spring force.

So we can see how is the contact between the seal and the lid and the groove, and the seal and the PEEK ring, and the PEEK ring and the metal groove. And then we release everything at the end so we can see and estimate if there are some kind of permanent deformation.

This is a short video just showing how the simulations are going to be. Where we can press down the lid, we activate the seal. We apply the hydraulic pressure and the spring force inside. So you can see the seal is moving and pressing on the PEEK ring. And the PEEK ring is pressing on the metal groove and keeping the seal inside the hatch.

We make a special inventor assembly. And this contains of the lid, the metal groove, and the seal, and the backup ring. So it is an assembly containing of four parts. And these four parts we will use for the simulation going into the Nastran.

Here is a smaller cross-section of the simulated assembly. And here we have the metal lid. We will apply an enforced motion to the lid. We have the PEEK backup ring here. And we have the PTFE seal.

And we have the fixed constraint seal groove here where we will apply the pressure. The seal, we have divided the seal into where split the surface. So we can apply different constraints and loads on the different areas of the seal.

This is a very small piece of the assembly where we have taken out 0.5 degrees or 1 degree angle slice of the whole assembly. And this is the part which we will use to apply into the Nastran. And where we will make the simulation on this one. So again, the enforced motion lid, the PEEK backup ring, the PTFE seal, and the metal seal groove which will be constrained fully.

So this is the seal again where you can see we have divided the surface here into different sections. So we can apply a spring load into two of the sections. And we can apply the hydraulic pressure into the areas where the hydraulic pressure will be running.

When we have the assembly, it's very important that we place the whole assembly. We place it in the zero point of our system, our coordinate system. So we use 0, 0, 0. So we have a fully control about where our parts are inside the coordinate system.

All the different parts, we constrain them. So we have a small distance between all the parts. They are not touching each other before we go into the Nastran. So we have a clear idea about where the different surfaces are in relation to each other. So we don't have any surface contact.

The analysis method and the coordinate system and material set up. So here we will first go into the Nastran. The Autodesk and then to Nastran by pushing the environment. And go straight into the Nastran software. And the Nastran software will be starting from that point.

The first thing we do when we now are inside the Nastran simulation software is we choose Analysis. It's by default put to Linear Static. We will right click on this one and go down and choose a Non-Linear Static Simulation for the whole simulation of today.

Because we had a slice of a round cylindrical part, we will choose to create a new coordinate system. We will not use the standard coordinate system down here. So we'll take the coordinate system and add a new one by right clicking.

We choose a cylindrical system. And then we manually put in the coordinate points for our cylindrical coordinate system. We start here at .000, which is where we put the path originally.

And then we apply directions to the main coordinate system where we have the angular and where we have the z-axis. And then we can use, it will come down here when you applied in the new coordinate system. And here we have just enlarged so you can see that the circular is actually going around in the right directions.

The material data for the three different solids-- we have the three different solids. The material part up here and down here. We take as a stainless steel. So first we choose to put the coordinate system, we have to choose the cylindrical system.

After choosing the cylindrical system, we choose that we have the seal groove and the top plate, so these two parts here. And then we choose to select this material. It was stainless steel already in Inventor. And he will adopt this material in here because the stainless steel is a material which is already in the database system of the Autodesk material database or the Inventor material database.

So all this information we need, they are already in because they are in the system. And here we just apply the solid and we call it stainless steel.

The next material we will apply is the PEEK material. And this is solid number three, so the green one. And again we have to choose the cylindrical coordinate system we apply at the PEEK ring.

Then we go into the material database. And then in our system we have the PEEK ring. So we select the material and choose the selected material. And we get this sheet here where we have the different material data libraries.

And we ask to load the database. And database is something we have created in our company. And here we have information, this is for the Victrex PEEK 450g. And we load this into our system and we get all this information automatically coming.

When we have these materials here, the sheet with the basic information about the PEEK, we can choose or push on this nonlinear button here. And we get this sheet where we can choose between four different methods of nonlinear isotropic materials.

In this one here, we have chosen a plastic which gives this type of curve. So we have the straight strain data which we got from Victrex. And when we ask to show all this data, we have just the pin put in. And here we get the curve. And this is the curve which the system will be using. So we have a straight line here up to the yield point. And then we have a very high plastic deformation after that point.

And this is what we more clearly can see here. The plastic, he has a straight line-- actually from 0 up to the yield point. So the yield point here defined as 95 megapascals. And then we have a plastic deformation after this point. So this is what we will use for the PEEK.

These are the data that we got from Victrex in the UK. And Dr. John Grasmeder, my old friend, kindly provided me the green curve for the stress strain data from the PEEK material. And we calculated what we call the true stress strain data, which are the data we have applied into the material database here.

The last material, the PTFE part, we do the same. Choose the cylindrical system that we applied in the PTFE seal. And then we go in and find again the material which we have already uploaded into our material database.

And in this case here, it's again isotropic material. We are using here nonlinear elastic material. So we have both compressive and tension inside these. And these are the data we have added in through the system.

And here we see again all the data we have put in from measurements we have been doing. We show the xy here. And here we have the compressive area of the curve. So this is when you compress the PTFE material. And this is when you extend the PTFE material. These are the data, which the Nastran will use for the calculations.

In this case here, we are on the material basic sheet. We ask the system to use the principal stress as a failure theory. So we can use this data. When he surpasses this information, it will automatically say it fails.

These are the data that we have been using for the PTFE. This PTFE is filled with carbon fiber, 10%. And we have the green curve. This is what we have been measuring in the lab where we have engineering stress strain data from compressive up to a tensile strain. And this we have been calculating from the engineering data up to the true stress strained data. And the true stress strained data are the data that we have put into the system.

So now we have all these solids which we need, so the idealization. And we have the stainless steel, we have the PTFE with carbon fiber and we have the Victrex PEEK. So now we have all the basic material information ready.

When you are working with your own material data and you have to find them yourself, measure them. This is basically what you need to run a fairly simple FEA.

You need the specific gravity. You need reference temperature. You need elastic modulus in tension and compression. You need the Poisson's ratio. You need the tensile limit, your compression limit, yield limit, tangent modulus, and thermal expansion coefficient. This is what you need to make your own material data.

These are the three samples which we are using basically for our first investigation of a material. There is the tensile test bar, small bar here for thermal expansion. And this is for compressive testing of the material.

This is the typical tensile test for a virgin PTFE. So it's a different material that we will also simulate with this one later in the presentations.

The compression tests here we typically compress it down to a minus. So 0.4, so 40% compression of the height of the billet. And measure the force we need to do that and calculate the stress.

Thermal expansion, we have the spatial bar very small. And we measure here from -22 plus 120 degrees Celsius. We measure the physical length of the part. And from that point, we calculate the thermal expansion quotient.

This is the typical tensile stress strain curve. This is from the PTFE with carbon fiber. So this is the engineering stress which has been measured in the lab. And then we calculate by this recognized method here the true stress strain. You can also measure true stress strain, but it is very complicated equipment you need to do that.

When we make a material data for simulating Nastran, we typically are making the test for the tension and compression. And we are using three different temperatures-- so 248 Fahrenheit, 73 Fahrenheit, 5 Fahrenheit.

And here you can see the difference on the same material. The blue one is the cold one, the green one is the room temperature, the red one is the elevated temperature material information. And you can see it's a big difference. And it's very important that you recognize that when you are simulating.

We are using what's called the strain rate of 0.01. So we are testing so the deformation is running what I would call fairly slowly. Which is for first simulations, to my opinion, a good idea.

Then we go in to set up further the case. So this set up on the Nastran, we need four different subcases. And initially we will just set up three subcases-- so subcase number 1, 2 and 3-- by just right click and New. And then we have all these three because these three will have the same, share a lot of information.

So here we make the constraints. So again when we choose to constrain here, we choose the coordinate system. This is important that we are running in the cylindrical system. And we choose Fixed. We fix everything.

We choose here the Surfaces. So the surface we fix on the sealed groove. These two surfaces, we fix them completely so we can't move anywhere. And then because it was already defined, three subcases. So I can then apply all three subcases to have this constraint.

The same we do with the cylindrical constraints. We use again the correct coordinate system. We choose all the side surface here and say we have symmetry. So we choose the symmetry around the [INAUDIBLE] And then it shows these three settings as fixed. And then I choose again the three different subcases. So we set up all three subcases at the same time.

The motion constrained because we are running enforced motion. So in the simulation, we will move. This oval lid, we move it down a certain distance. We need a constraint on top of that with the cylindrical system.

And here we choose just one direction, down, to fix that. And this is the surface. So we take the whole surface on the lid and all three subcases we need this because we will make enforced motion in all three subcases.

All constraints are now defined and will operate in all three subcases. That's why we set up three subcases from the beginning.

Then to contacts. We have to identify the contacts between all the elements who are in touch or who will touch each other.

And I'm always using the manual setup. So I choose the manual setup. I choose the separation. I'll choose unsymmetrical penetration type, meaning that the primary entry will be the stiffer part. And the secondary entry will be the softer part, so the flexible part. And this is the non-flexible part.

For a number of reasons that we will come back to, we have chosen the [? correction ?] of friction. We have eliminated it or put it at 0. And we make activation distance automatic. We'll just push this to the bottom here.

We select the harder surfaces, the lid, and the softer surfaces, the PTFE seal. And these are all these surface areas here we are defining as the softer part.

However I just took this top part on test visibility, so it disappeared. It's still in the simulation. But I can see now if I go into the surface contact I can see the blue is the hard part, so this one here. And the red ones are, this one's on the [? ceiling. ?] So these are basically just you can see that you have added the correct one.

We do all this with all the different contact areas. So we have on the bottom here, we also choose this part of the PTFE because everything will be in contact with the bottom groove. This is the same on symmetric hard material, soft material and no friction.

This is the same. We are using also between the PEEK and the PTFE. All is the same. And we use it between the PEEK and the lid. And this is the surface contact here between the PEEK and the groove, the ceiling groove. So we have now defined all the surface contacts.

The loads, we have to apply some loads. And here we have the three different subcases. We have three different loads scenarios in all, or actually in four subcases because we will add a fourth subcase later. We push the load.

And here we have to choose the cylindrical system. We choose an Enforced Motion. And again this Enforced Motion we need to apply. In the first three subcases, we have put here a distance. And this is going down as 0.15 millimeters, which is in inches 0.006 or something like that.

And we choose as the Enforced Motion and we do it in all three subcases. So we have to do that. We have to choose the cylindrical system. And now the lid will move down in the first subcase. And this is the only thing we're doing in the first subcase.

In the second subcase here, we apply another Enforced Motion. And the same cylindrical system, now we apply -0.3. So now we have a 0.3 in the second motion and first we have 0.15. And you have to add these together. So in total, it will be moved down -0.45 millimeters.

And these apply only to subcase 2 and 3. And again, we choose the surface here on top of this one. We can choose also the bottom surface, but just one surface and the direction will do there.

So we have this Enforced Motion. It goes in subcase 1, 2 and 3. And Enforced Motion 2 is only valid in subcase two and three.

So here we apply again in subcase 2. We apply this as spring force or we miss the metal spring. So here we have applied pressure. So we take normal to surface, we take pressure here. We apply the magnitude of the pressure, 0.75 megapascal. It's about 108 PSI. And this is applied in subcase 2 and 3.

Subcase 3 we add on top of all the other loads. We apply another pressure of 10 megapascal, like 1450 PSI, on all the inside surface-- almost all the inside surface-- of the PTFE. And this is valid only in subcase 3. And this is the hydraulic pressure which will activate in subcase 3.

Now we will make subcase 4. In subcase 4, we just duplicate subcase 3. This gives us all the same constraint and all the same loads. But it gives us a copy of the load. So this load, we can change the numbers in the copy without changing the numbers in the first three subcases. So I think it's a nice way of doing it.

You get it all automatically, but you get it as new constraints and new loads. And this you can change as you like. So we remove all the forces of the Enforced Motion 1. We simply just remove this. We just need one Enforced Motion to go back to 0.

Here we have the hydraulic pressure copy. We put it to 0 pressure, so we remove all the inside pressure. Here it is gone. We take Enforced Motion 2, we take it to the magnitude. And this is the relative nature of 0. So we put the lid back to the 0 position.

Then we have Meshing and Mesh Control. The mesh, the Nastran will suggest you some kind of mesh size. And typically I will have a look if how it fits through the cross-section of the parts.

And in this case, I like to get it a little bit finer than what it takes. So I take it down to 0.519 instead. And then we make what is called a mesh control of 0.3035. And the mesh control we do only on the PEEK ring and on the PTFE ring.

So the two major parts, it's fine with the coarser mesh. It's run faster and it's OK because we don't have any deformation in this area. So we are only interested in the PEEK and the PTFE.

For the mesh control or mesh system, we are typically using an Excel sheet where we put in the value, which we say this is the suggested value of what we choose as a first starting point. And then we can calculate if we want to make it finer, the mesh, or we want to make it more coarse.

And then this Excel sheet here will calculate the different mesh size for us. And we're using this to figure out how many elements, nodes, what are the stresses we get, and then we estimate the wall clock time.

So how long does it take the software to calculate? And will it run, will it complete at all? And this we are doing to find the better balance between the time of the simulation and the correctness of the results. So if you get better results.

Nonlinear setup, we need to-- All subcases, we have a nonlinear setup. And we need to change all those. Or not change them, but in the intermediate output we will choose. It's standard set to Off. And we set it to All so we can see. It will update the graphics during the simulation so you can follow how it's working through.

And then we have some parameters we can choose from. On the bottom of the tree, we have parameters where we can go and set different parameters if the default are not OK. And here we are choosing contact stability. It's called CONTACTSTAB. You need to check this advanced settings box.

And you just search here, he finds it. It's default put to auto. And typically it will be off running. And we choose here to put it to On because we need to stabilize the different contact points.

The contact points, these are between the nodes. And we have my friend David who will explain to you about the contact step, the description of what it's doing and how it's basically working.

Now we are ready to run. And it's just hitting the Run button here. And then we will start the simulation.

Now we run the analysis. And the analysis will complete. In this case, it completed in the first one. It's not always the case, but here we were lucky. And you can see down here, completed load 4.0. So 4 subcase, you went to the end. And there we can estimate how it is working.

We need to change the plot. So you put this option here, push this one. And then you get the plot. And here we will, under the control, specify minimum, maximum. So I specify the axis here going from 0 to 20 megapascal on this one. And then I basically always have this as twice as much as this one, so 40.

And then I push the plot and I get a replot where the colors are reassigned and the bar is going from 0 to 20 megapascal. This makes it possible to compare all the results all the stress levels. You can compare from the individual subcases. Subcases we have loaded differently and of course, we will get a different response.

So here we have afterload case number one, where we just moved the upper lip down to get into contact with all the parts. And here you can see it's just starting. And of course we are at almost 0 stress.

Subcase 2, we put the lid down in the correct position and we applied the inside pressure from which [INAUDIBLE] the metal spring. And of course now we get a lot of stress inside. We apply the hydraulic pressure inside the seal. The reason we did not apply it outside here, the pressure, is because we have the same pressure on this side and this side. So we just say, for the simulation purpose, we don't need to apply pressure on that area.

And this is after subcase 4, where we see the lid is back. All pressures are released. We still have some indication of stress inside here. The stress is because we have a small permanent deformation. And the software calculates if we have deformation, we have stress. But the stress will be 0.

This is a small movie showing how we are looking at the different subcases. So here we have only enforced motion. And when we go to the subcase, basically it's just what you have been seeing. And we push up there at the end of the subcase 1 and we see that it's moved down.

And we have now contact between all the parts almost. Not the PEEK, it is still floating freely between the seal groove and the PTFE seal.

In subcase 2, we have the spring. We have the two enforced motions. So now we have pushed it down -0.45. And we apply the spring force inside our spring pressure inside the metal seal. And here you see now we gain some contact in this area here. So we have a sealing contract already now.

And it will go on to the next one, subcase 3. And here it is spring pressure. It is hydraulic pressure, enforced motion 2 and 1. So these are all the four loads applied at the same time. And here we can again see how it's looking after the different number 1. This is after number 3, sorry.

So here we have a lot of pressure. We have a lot of contact. Everything has been squeezed out. You can see here the original shape of the seal. So all the seal have expanded on the diameter. We have a high load outside in the hatch roof.

And after releasing the pressure, everything is run to 0. You can see down here it shows we put all parameters to 0.

And here everything is released back again. And we are having some permanent deformation, a little bit you can see compared to the original shape. The seal is pressing the PEEK ring out.

And here we have been running the same simulation but with a different material. This is the PTFE. The virgin PTFE will be running.

So you can see the-- It's the same deformation where we have applied the spring force. And this is showing that you have still a good contact here.

And here we applied the full load. So when you see very heavy deformation on the seal lips and [INAUDIBLE] because the material is much more softer. And still we have a very big contact at the end of the seal now.

And this is after reloading. Where with a softer material, we see very big, permanent deformation on the seal. The seal has expanded, still pushing on the PEEK ring. So he expands the diameter, lips are getting smaller. This is exaggerated compared to real life. But this shows you that it is worth having a look on the simulation.

We are running the analysis with different mesh sizes. So we have, this is the original mesh size we start with for all parts. And then what we are doing is that we are changing the mesh to see if it runs faster, if we get less failures or less warnings.

And we see how the stress level is going. The stress level should be smaller and smaller, which is better and more accurate. The higher stress we get, the more inaccurate the simulation is.

This is a mesh size where we have used a very coarse mesh. We still have the same with the friction. And here we have a fairly higher stress in what we were having in the video you just saw.

Here we look at the wall clock time. You can find on the Nastran page. Wall clock time-- we monitor this because the faster it gets, the faster the system is running. We look at the warnings, we have about four. We like to have zero, but four is very fine. And no fatal errors.

We changed here the mesh. So here we have mesh control. So the seal and the backup ring, we have also a coarser mesh than in the first simulation you saw. And again here we have a little shorter wall clock time. And we have the same amount of warnings but much, much higher stress in the area. So this is not a good indication for this mesh.

Here we took the mesh. We keep the mesh, general mess. And we reduce this one. And our wall clock time is going up. We still have the same warnings. And then the maximum stress is going down. So it's indicating that we are having a better simulation.

We have been running with different combinations of the basic mesh and the mesh control. And here we monitor the nodes and elements.

How many do we have? What kind of freedom do we have in the system? Our degree of freedoms. And in this one here, we have now increased the wall clock time. The warnings go up a little bit. And even the stress goes up a little bit. So we were running with a bigger mesh and this is not good.

The same here. We have now increased the mesh even more. And the nodes and elements goes very down. And then we have a very fast time, 136 seconds. And we still have four warnings. And the size of the stresses, it could be OK. And it's on its way down, so that's a good sign.

And this here is even more coarse. We have 115 seconds of wall clock time warnings. We only have two warnings. But still we have a little high. The basic picture on the seal looks to be OK. But on this part here we had when we turned the part around, we have this small part here is sticking up.

And this is a node which has penetrated the surface on the counterparts of the metal. This node is actually inside the metal bar. And this is of course wrong. And this we like to avoid by changing and controlling the mesh and also controlling the situation around the frictions and so on and so on.

Mesh, the aspect ratio of the mesh is very important. And it's very important that we have. And this is what David will explain in more close details during the live presentation.

We have different types of aspect ratio which we have to control. One important thing is the mesh should fit. So if you have the blue is the figure and the green is the mesh, the mesh does not fit very well. And this is what we like. In all kinds of shapes and colors, we like the mesh to follow as close as possible.

Final, we have run 1 and 2. Run 1 and 2 is where we change the piece of PTFE material. So the first one, we chose the carbon fiber filaments here, the data from before. And we have the starting point. You see we have subcase 1 touching. And then we have applied the small pressure inside. It's what you have seen before.

In subcase 3, where we have all the pressures inside and the motions and then we release it in here, we see only very, very small differences from the original shape. The PEEK ring likes to get up because it's pushed out by the PTFE seam.

And what we did is we changed. Now you can see here the difference between the end of subcase 4. And this is the beginning, before we start. So you see the difference-- not very big, but that's a little bit.

Then we change the material to a virgin PTFE called TF1620 with data we also had. And here we have subcase 1, that's where we start. 2 looks normal. 3 same as subcase 2. Sorry, same as before.

Contact, no more stressors on them. And then we apply the pressure. The pressure is better distributed in this material because the material is floating. It's deforming.

And then when we release it, we see a very heavy plastic deformation. This is exaggerated compared to real life. But it shows us that this material is stressed out beyond the heat point. And we should consider, if we use this in the real application, using a different material as the first one.

So here again you see the starting point and after subcase 4. So there's a very big difference. This is because it's a softer material. And this is why we are simulating, to illustrate these kind of things.

So these are the PTFE-- 10% carbon fiber and the virgin PTFE. So you see here full pressure. We have a better sealed surface on the harder material. And more it is still a sealed surface, but it's the same pressure almost all over. We don't like that. And then we have the heavy deformation on the virgin PTFE.

So we are now happy to answer your questions if any one of you have some. And then at the end, we say thank you a lot for your attention.