You will get large (in terms of absolute value) stresses at the ends due to boundary conditions. Did you try solving this in plane strain or with solid elements ? Is the mesh sufficiently refined ?

Screenshots of the model could be useful to provide help.

Sure thing! Attached just 2 snapshots of the model in wireframe and smooth shaded.

To elaborate, there are 100 elements down the length of the model and 100 elements that follow the circular path. So it ends up being 10,000 elements used.

I thought it was interesting that the von Mises stress it shows was much higher than the x-component (tangential direction). I also figured the stress would vary towards the ends due to the boundary conditions, but was confused to see what I thought would be a purely tensile load cause extremely large compression numbers towards the ends.

The elements used are 2D Shell elements. QUAD4 in particular.

That's a very fine mesh, no need to further increase its density. However, as I've mentioned, I would try with other types of finite elements. Maybe you will also be able to apply different boundary conditions that don't overstiffen the ends of the pipe. But this depends on the real-life support conditions.

Yes, the mesh is indeed pretty fine. It is set up that way because of the number of data points needed from the output of this analysis.

Thanks for the suggestion. I will experiment with some other elements. I have just read that 2D Shell elements tend to be quite good at idealization for thin-walled pressure vessel types of models.

I have thought about the boundary conditions a bit. For its use right now, the boundary conditions aren't rigidly defined. I think I have seen someone recommend only restraining a single point for an open-ended pressure vessel type problem.

Shells are indeed the right choice for thin-walled structures like that but in some cases they are insufficient.

You could also utilize symmetry in this model to solve it faster and to make boundary conditions less problematic (unless the loading is unsymmetric of course).

Update:

Tried this 3-2-1 method of constraining the model found in this forum that seemed to work for other people.
https://www.eng-tips.com/viewthread.cfm?qid=176220
https://www.eng-tips.com/viewthread.cfm?qid=178234

The stress found was uniform throughout and in a positive realistic value range.

The only issue now is that pressure seems to be governing how much the stress changes rather than temperature. What I mean by this is that changes in temperature seem to have little effect on the stress values seen in the results. This should not be the case, especially when there is temperature of 1000 deg F applied. The stress values I am getting now are too low. I have used a Coefficient of Thermal Expansion that handles units in Fahrenheit and have assigned Fahrenheit values to the temperature loads.

So, now I have to try and discern why that might be.

Double-check the input values and make sure that all units are correct, that’s often the cause of wrong results in such cases. What about the analytical solution - how does it compare to the values you get with temperature included ?

Thermal stresses are very sensitive to boundary conditions. Try the approach with symmetry, it might give you better results.

When you say symmetry, do you mean turning the 3D problem into a 2D one? Or just cutting the problem in half. I understand people take symmetrical geometries/loads and will sometimes cut them in half to reduce complexity of the problem.

Also, I have the pressures applied to the internal face of the element and the temperatures applied to the nodes. As far as I know, that is fine, but I could be wrong here.

Not necessarily 2D (although I would try plane strain too). You can utilize planar symmetry reducing the model even to one-eighth. You just have to apply symmetry boundary conditions to the edges or faces of the cut. Many FEA codes have predefined BCs for that, in others you have to manually select proper degrees of freedom. In 2D symmetry would also be helpful but you would have one direction less to worry about.

Yes, that’s correct - distributed loads are applied to the faces of the elements while temperatures are defined for nodes.

Check the reference temperature definition too, it’s important in thermal stress analyses.

The analytical solution is about an order of magnitude higher than the FEA results. Which makes me think there is an error with inputs. Alas, the inputs were double-checked and were correct.

Currently, I have the reference temperature and the initial temperature both set at 70 deg F. So, I expect it to expand plenty at the higher temperature values, but this does not seem like the case.

I see that I can set up the material properties as a 2D Solid for the plane strain responses. Going to try that and see what happens.

Thanks for your help!

You should not completely fix the ends of the column. If this is continuous pipe or connected to any other pipe by flanges or connected to equipment, making use of cylindrical co-ordinate system based boundary conditions would reduce the stresses. You need to fix only theta and axial translational degree of freedom and free the radial translation direction (for solid elements) as radially the pipe is free to move(Unless not completely blinded off or attached to stiff structure which would not allow radial movement). Still the stress values would be expected to be much higher due to the temperature and axial restraint provided at the end (Thermal stress). But I would not worry about those as these are secondary in nature and higher allowable stress can be used (See ASME Sec VIII Div 2)

Update:

Was going to try the plane strain, but tweaked a few more parameters and ran it with the 3-2-1 BC.

Stress induced by the pressure in the tangential direction (Hoop Stress) has a 0.05% error between theoretical versus FEA results. NICE!!!

Varying the temperature causes no change in the tangential direction stress. (i.e. 100 deg F and 1000 deg F cause the same amount of stress, which is likely calculated to be zero in the FEA, with an initial temperature of 70 deg F and reference temperature of 70 deg F)

So, does anyone know why a large temperature difference (such as 1000 degF from 70 degF) causes no stress in the model with a Coefficient of Thermal Expansion of around 5.11 microin/in-degF ?

As I've mentioned, thermal stress analysis results are particularly sensitive to boundary conditions. You have to make sure that they correspond to the assumptions of the analytical solution.

Can you share the complete data - all dimensions, material properties and prescribed values as well as the formula used for the analytical solution and the result of it ?

Ro: 0.233 in
Ri: 0.172 in

When constructing the geometry, averaged these to get the midplane radius and applied thickness in material properties.

R: 0.2025 in
L: 0.9320 in
t: Ro-Ri = 0.0610 in

Meshed with QUAD4 elements (100 around the circle, 100 down the length)

Material Properties of Ti-6Al-4v
E = 16500000 psi
Poisson = 0.33
Density = 5.14784 lbf/in^3
CTE = 5.11E-06 in/in-degF
Reference Temp = 70 degF

Load Cases (internal pressures on element face and temperatures on nodes)
P3500_T-400 P3500_T-330 P3500_T-260 P3500_T-190 P3500_T-120 P3500_T-50 P3500_T20 P3500_T90 P3500_T160 P3500_T230
P3500_T300 P3500_T370 P3500_T440 P3500_T510 P3500_T580 P3500_T650 P3500_T720 P3500_T790 P3500_T860 P3500_T930 P3500_T1000

P100_T300 P440_T300 P780_T300 P1120_T300 P1460_T300 P1800_T300 P2140_T300 P2480_T300 P2820_T300 P3160_T300
P3840_T300 P4180_T300 P4520_T300 P4860_T300 P5200_T300 P5540_T300 P5880_T300 P6220_T300 P6560_T300 P6900_T300

Quite a few load cases... held T constant and varied P. held P constant and varied T.

Formula for checking pressure induced tangential stress (Hoop Stress)

@ 6900 psi P_i
hoop thick = 26355 psi
hoop thin = 22906 psi

(FEA shows stress for this as 22894 psi)
hoop thick ~ 13% error
hoop thin ~ 0.05% error

This tells me the FEA arrives at the same answer as the thin-walled result.

Formula for checking temperature induced tangential stress

@ 1000 deg F and 70 deg F
thermal stress = 67270 psi

FEA essentially says this is zero. (i.e. same pressure but different temperatures give the same stress)

Your input data looks correct. However, the key here is to clarify which variant of boundary conditions you assume. Do you want to allow the pipe to freely expand in the axial direction or should it be fully restrained at both ends ? This will determine what thermal stresses you get as a result and what analytical solution you should use. Is the purpose of this analysis to simulate the behavior of a real structure or is it just a theoretical consideration ? What is the source of the analytical formula you are using - does it come from some book ?

If there is no restraint on the pipe, and the temperature field is uniform there will be thermal strain, but zero thermal stress.

I added the 3-2-1 method of constraints on both of the ends. This works out to 6 constrained points.

The stresses vary through the length of the pipe like you would expect. However, the stresses are still not as high as I calculated.

Thanks SWComposites, I see that now as I have played with it a bit more.

FEA way, I suppose that is where my issue lies. I thought it would be simple to completely fix both sides because I have no specific boundary conditions yet, but I know that the minimal constraints are not sufficient for the thermal aspect of the problem.
I quickly worked out the thermal stress formula from the only source I could find. https://www.nrc.gov/docs/ML1312/ML13127A280.pdf
This gives a integral equation for it, but I worked it out to be something similar to what I posted previously. What are your thoughts?

Thanks for the prompt responses.

The 3-2-1 method is interesting but one has to keep in mind that it's meant for situations when you want the model to be rather "free-floating" and relying on the load balance itself but the software requires some constraints to eliminate rigid body motions.

For the thermal stresses to develop there must be some constraints (internal or external). It can be a fixed constraint on both ends (external constraint), a connection of materials with different thermomechanical properties or simply a temperature gradient. The analytical formula that you use assumes the latter cause of thermal stresses since it's meant for nuclear reactor pressure vessels. If you look at the boundary conditions described there, the following assumptions are made:
- inside surface - convective heat transfer with hot water flowing in the pipe
- outside surface - zero heat flux (insulated)

mtz_engr

Quote (NRP99)

You should not completely fix the ends of the column.

Read "pipe" instead of "column". I am still not seeing any problem unless the boundary conditions are completely wrong. Perhaps a screenshot of stress results/boundary conditions would help to understand what is going wrong here. Or Perhaps little bit more background information is what I need to make proper suggestion like what part is this? How its exposed to this much temperature and with what medium? How the ends are restrained? etc. etc.

What I stated about boundary conditions and stress evaluation in my earlier post is normal way of solving the problems in Pressure vessel industry. If this is applicable to you, it should solve your problem.

D/t ratio is (0.344/0.061)=5.63<20 means you cannot approximate to thin shell approximation or shell modelling approach. It is ok but 3d solid modelling will give somewhat better accuracy as its thick shell.

This is supposed to be a generic component used in liquid rocket engines. The pressure and temperature data is taken from one engine in particular as an example of loading environment. These temperatures are given to be what temperature the inner wall experiences after heat transfer has been considered from the moving fluid. I am trying to solve a generic case that would be formulated early in the design and use that many load cases as a means of forming a stress distribution from the data.

The problem with it being a generic case is that the boundary conditions aren't explicitly decided yet, which I understand will definitely affect the stress. The idea here is to determine what the distribution of the stress would look like at this range of loads when the component has been designed based on the analytical results + a factor of safety consideration.

I am struggling to determine what boundary conditions would work for my problem. If it is constrained too much, there are issues. If it is constrained to little, there are issues.

I will try the 3D solid modeling approach, but I still believe you both are correct in suggesting the boundary conditions are the real issue here.

The equation that the OP has posted for the thermal stresses in the hoop direction are derived with the assumption that there is a temperature gradient through the wall thickness of the cylinder. Your FEA does not model that. You have a zero gradient (constant temperature) across the shell thickness and you use rigid-body constraints (free-free ends) so naturally you get zero thermal stresses.

Try modeling the temperature gradient through the shell thickness with rigid-body constraints applied. This should model your problem based on the theoretical formulas you have provided.

Okay! I took a stab at your problem. I've taken the case where:

p = 6900 psi
Ti = 1000 degF (on the inner surface of the cylinder)
To = Tref = 70 degF (on the outer surface of the cylinder)

For a temperature gradient in the radial direction, assume that Ti and To are the uniform temperatures at the inside and outside cylinder surfaces respectively, and the temperature variation across the wall thickness is linear. The stresses in the hoop direction at the outer surface of the cylinder away from the edges are taken from Timoshenko’s text on Plates & Shells as:



The symbols have their usual meaning. Here t1 = Ti and t2 = To. Hand clac’ed values are:

Shoop(thermal) = 59 ksi

Now using the thermal stress formula which the OP had quoted earlier and with the values provided, I get:

Shoop(thermal) = 64 ksi

So, its comparable with what Timoshenko gives.

The max thermal stresses will be on the outer surface in the hoop direction at the free-edges given once again from Timoshenko’s text as:



Hand-calc’ed values are:

Shoop(max_thermal) = 71 ksi

When these results are superimposed over the pressure case, we have:

Shoop(total) = Shoop(max_thermal) + Shoop(pressure) = 71 + (6900*0.2025/0.061) = 94 ksi

The location of the max stress is at the free-edge.

Modelled the cylinder using CQUAD4 shell elements using MSC.Nastran. Made a coarse mesh of just 20 elements across the length and circumference. Defined the temperature variation across the thickness of the cylinder using the TEMPP1 card. An internal pressure of 6900 psi is applied using the PLOAD4 card. Used the same dimensions and material properties as the OP has quoted before. Boundary used are free-free at the ends and just the rigid-body modes suppressed. Ran it for the combined pressure + thermal case.

Compared with FEA:

Shoop(total) = 94 ksi (Theory)
Shoop(total) = 93 ksi (FEA)

Below is the stress plot from the FEA showing the hoop stress on the cylinder outer surface.

@nlgyro

That is fantastic! A few follow ups.

I was wondering how to consider Thermal Stress as a function of the geometry (Ro, Ri). That is how I found the original equation I used. I suppose it is not 100% necessary as the results you obtained and the theory line up quite nicely.

Can I ask how exactly you constrained the model? You said Free-Free ends with Rigid Body Motion prevented. So does this mean you constrained the z-direction and all rotations?

Also, I can't find any resources for how to apply the TEMPP1 information (i.e. the linear gradient) to my model in Patran. Would you be willing to explain it or point me in the direction of good resource?

Thank you and great work!

Quote (mtz_engr)

Quote (I was wondering how to consider Thermal Stress as a function of the geometry (Ro, Ri). That is how I found the original equation I used. I suppose it is not 100% necessary as the results you obtained and the theory line up quite nicely.)

Well... this is pretty easy to do if you’re modeling your problem as a 2D plane strain or as a 3D model.

To consider the thermal stresses as a function of geometry you must create the nodal temperatures as a function of the geometry (radius in this case)

Let us assume a linear variation of temperature across the wall thickness of the cylinder of the form:

T = To + (Ro-r)/(Ro-Ri) *(Ti-To)

where:
T = Temperature at a given radial distance 'r'
Ti = Temperature at the inner wall
To = Temperature at the outer wall
Ro = Outer radius
Ri = Inner radius
r = given radial distance.

You can use the Create--> Spatial---> PCL Function option in the 'Fields' menu of Patran to enter this equation. The FE-model needs to have all the nodes associated to a radial co-ordinate system for Patran to pick up the radial distance of a given node in your model.



So, give a name for your field under "Field Name"
Use the Field Type as "Scalar"
Co-ordinate system type as "Real"
Under co-ordinate system select the radial co-ordinate system that you have created. (The coord 100 that you see is the radial co-ordinate system that I had created.)
Now considering the temp and geometric values in your example the equation in Patran would be entered as:
70 + (0.233-'R)/ (0.233-0.172) *(1000-70)
under "Scalar Function". 'R is the Patran convention for the nodal radial distance.

Now in the Loads menu under Create--> Temperature ---> Nodal under "Input data" select the above created field in the 'temperature' box. Click on the "Select Application Region" and select all the nodes in the model. Hit Apply for patran to interpolate the nodal temperatures. Once you run the model you'll have the variation of thermal stresses across the thickness.

Now the model that I did was a plane-stress model using 4-noded shell elements. The temperature interpolation across the shell thickness was done using Create--> Temperature ---> Element Variable. In the input data you just enter the top and the bottom surface temperatures which would be To and Ti respectively. In the Select Application Region, just select all the shell elements. This automatically creates the TEMPP1 card which contains the parameters for Nastran to do a linear interpolation across the shell thickness. Refer the nastran quick reference guide for more details on the parameters of the TEMPP1 card.

Quote (Can I ask how exactly you constrained the model? You said Free-Free ends with Rigid Body Motion prevented. So does this mean you constrained the z-direction and all rotations?)

There is a standard way to do this when modeling cylinders/pressure vessels. Follow the slides in the attached pdf.

https://res.cloudinary.com/engineering-com/image/upload/v1641894801/tips/RBE3_Example_ojmo50.pdf

Quote (Also, I can't find any resources for how to apply the TEMPP1 information (i.e. the linear gradient) to my model in Patran. Would you be willing to explain it or point me in the direction of good resource?)

Explained above. General rule... for description on all nastran cards use the nastran quick reference guide which is available in the nastran documentation folder along with the software installed on your PC. Version of the quick reference guide are also available online in the MSC website.

From the load-cases that you have posted earlier looks like you are dealing with super cold and super hot fluid conditions. This means at some stage in your analysis your mechanical properties such as E, G, nu and alpha would have to be considered as functions of temperature. The MATT1 card in nastran comes in handy for this.

Good Luck!

Good nlgyro.

Quote (nlgyro)

There is a standard way to do this when modeling cylinders/pressure vessels. Follow the slides in the attached pdf.

I would recommend to use datum cylindrical coordinate system and apply theta and axial constraint at the ends directly as stated in my first post rather than doing whole RBE3 exercise.

Interesting slideshow on RBEs. I am not sure I fully understand what it is saying though.

It looks like it is saying make 3 nodes the independent terms in an RBE for all 6 DOF, then, for every other node, make it the dependent term for those three independent terms in all 6 DOF.

That must not be the case, because I just tried it and received an error.

Could I not just constrain the entire side in rotation and axial directions to achieve a similar result? Or does that add stiffness to the model.

Hi everyone,
I design reactor with partition plate divided the reactor to two separate reactor. one side the design temperature is 350 centigrade degree with 3.5 bar internal pressure. the other side is empty and under ambient temperature. I want to design the partition plate but under this gradient temperature the stress is two high in the place of contact the plate with shell. I use FEA with ANSYS . the stress is 4000 MPa. I model the partition plate and a part of shell with internal pressure and convection for thermal. I think my model has a problem that the stress is two high. when the stress linearization based on ASME sec viii part 5 in not pass. Could you please give me a advise?

Quote (mtz_engr)

Quote (It looks like it is saying make 3 nodes the independent terms in an RBE for all 6 DOF, then, for every other node, make it the dependent term for those three independent terms in all 6 DOF.)

If you look at slide 44 that's all you need! Just one wagon-wheel RBE3 at one end of the cylinder which connects the dependent node at the center to the independent nodes on the circumference. Use dof's 123456 for the dependent node and 123 for the independent node. Select 3-nodes 120degs apart on the circumference and add them in the UM nodes putting theta and Z dof's in the UM set. Add a SPC 123456 at the dependent node at the center. This method constrains all rigid-body modes and allows for un-constrained motion when you have self-equilibrating mechanical loads and thermal loads (such as an aircraft in flight) without constraining the model to ground. This is a generic way of doing it.

Quote (a prime example of GIGO)

@miningman

A lot of posters here tried to support the OP's question in a professional manner by spending their time in understanding what the OP is trying to doing with an intention of helping him out the best they can. None of them have taken cheap-shots! Why do you undermine the efforts of such people by labelling this exercise as GIGO?? Being your first post on this forum all that you have done is just post your typical arm-chair rocking/pipe-smoking condescending BS!! What a retard!!

Is it just me or should the moderator of this forum (if there is one) step-in to reign in these "Kids these days... Ho! Ho! Ho!" types??? I'm sure the internet is full of free un-regulated spaces where such BS flies!!

Thanks @Couch_King

If I knew everything, I wouldn't be here. Was fortunate enough to have some good folks that know this topic better than I do share their advice.

Very thankful to the people who share their knowledge here!

@nlgyro

So, the best I can understand this is to set up the center (20000) as a dependent node in 123456. Then add every point on the circumference to the independent set in 123. Then, to achieve a similar looking RBE3, add the three separate points that are 120deg apart to the dependent set in 36 (translation in Z and rotation in Z with Z being along the axial direction).

The center node has a SPC 123456 and it is the only SPC specified.

Does this sound right to you? Because I still seem to be getting errors once I submit the job to Nastran and check the F06 file.

Couch_King

I do not want to be rude but you made the same mistake of posting your first post with only rant not showing professionalism either. You can help forum without using derogatory words. I, to some extent, agree to the comment by miningman since lot of questions are based on input provided by analyst to software and not able to understand the software output they got. That suggest something, right?

mtz_engr

I would suggest to look at previous responses one more time. It seems you are trying hard in implementing the software procedure and without understanding the physical understanding of the problem. This would be not be helpful to you if you avoid understanding the problem physics before you try to solve in analysis software. Then you will get bounced by these sort of questions/errors every time you analyze any complicated problems.

Quote (NRP99)

Quote (I do not want to be rude but you made the same mistake of posting your first post with only rant not showing professionalism either. You can help forum without using derogatory words.)

Seriously!! You have this poster miningman(Mining) whose first post on this forum (before the comments were deleted) demeans and take cheap-shots at the efforts of the posters who have tried to help the OP with his problem by labeling the entire exercise as GIGO without contributing one useful bit to the discussion. Now this is derogatory and lacks professionalism. Plain and simple. It’s akin to making fun of someone who fallen into a swamp for having fallen into the swamp!! The least you can do is the help him out and then point out his mistakes. That’s decency. All I did is point this out in no uncertain terms.

Quote (I, to some extent, agree to the comment by miningman since lot of questions are based on input provided by analyst to software and not able to understand the software output they got. That suggest something, right?)

Well I don't want to sound rude either, but the introspection should start with some of the gems that you have belted out on this discussion.

Now this is a free site. If you are an experienced FEA user, you are welcome to stop-by and help other if you have the time and the willingness to do so. Otherwise you’re free to move on but don’t turn it into swamp just because some user asks a question too pedestrian or lacks the understanding of the problem he is trying to solve. People like me who use FEA very rarely stop-by at this forum just to pick-up tips and tricks from experienced users. The last thing we want is for the experienced users to flee this forum or to lose interest in posting anything because there is always some random user/users who contribute nothing but makes it a point to stop-by just take cheap-shots at other users who genuinely help the OP with his/her FEA problem!! I think the response by the OP underscores my point:

Quote (mtz_engr)

Quote (Thanks @Couch_King

If I knew everything, I wouldn't be here. Was fortunate enough to have some good folks that know this topic better than I do share their advice.

Very thankful to the people who share their knowledge here!)

I sincerely feel this discussion forum could be better moderated!!

Quote (mtz_engr)

You are almost there. Just use 23 dofs for those three nodes 120deg apart. This will do. See attached pic file.

• https://files.engineering.com/getfile.aspx?folder=e8f3037b-30e3-4d3e-9e38-f

How odd. I reconfigured the RBE3 to have the 23 DOF for the three nodes, but there is still an error.

In the F06 file, the OLOAD RESULTANT matrices for each subcase has approximate zeroes everywhere.

However, there are two sections with error messages. One concerning the UM set. The other concerning the matrices. (Attached photos for F06 text)

It seems like a DoF in the RBE3 is dependent on itself in some way. Thinking this could be a problem with the three 23 DOF nodes being in the dependent and independent sections?

Seems weird that I would receive this error if you are not and are performing this same operation.

Attatch your input file which FATAL's out. I'll have a look to see what's going on.

Ah. Well, after playing around with the coordinate system, I found that there were issues with the nodes RCID versus the ACID.

So, now I have achieved a similar functioning model to yours. I changed the geometry based on the Timoshenko equation during design.

At the Max P and Max T,

Hoop(total) = 86.3 ksi (FEA)
Hoop(total) = 93.6 ksi (Theory - Hoop thick formulation)
Hoop(total) = 90.1 ksi (Theory - Hoop thin formulation)

Mind you that based on the new geometry the theoretical formulation should be for thick version of the equation.

Based on that, we have around an ~8% difference. Wondering where that difference is coming from. I know the FEA isn't perfect, but would like to know how to account for that.

Questions

- where are these stresses measured? Outer/inner & middle/ends of the pipe??

- what are these new dimensions??

- same max pressure and max delta-temp as earlier??

Because I have modeled it as a 2D surface, I believe it is measuring it at the midplane (Ro-Ri)/2. I modeled it at the midplane because when you apply thickness to the material properties, it extends out in both directions (from what I have read).

I believe this is the source of error, because the FEA may be outputting the midplane values, while the theoretical results output the maximum value that is experienced at Ro.

Also, the maximum values in the FEA are on the ends, so that is the value being compared to theory.

New dimensions are 0.212 in and 0.133 in for Ro and Ri, respectively.
The midplane value that the geometry in FEA is created from is 0.1725 in.

Temp and Pressure values are still the same, yes.

Quote (mtz_engr (Aerospace)(OP)17 Jan 22 18:56
Ah. Well, after playing around with the coordinate system, I found that there were issues with the nodes RCID versus the ACID.

So, now I have achieved a similar functioning model to yours. I changed the geometry based on the Timoshenko equation during design.

At the Max P and Max T,

Hoop(total) = 86.3 ksi (FEA)
Hoop(total) = 93.6 ksi (Theory - Hoop thick formulation)
Hoop(total) = 90.1 ksi (Theory - Hoop thin formulation)

Mind you that based on the new geometry the theoretical formulation should be for thick version of the equation.

Based on that, we have around an ~8% difference. Wondering where that difference is coming from. I know the FEA isn't perfect, but would like to know how to account for that.)

I don't understand your argument of comparing thick-shell theoretical numbers to thin-shell results.

But considering your new dimensions and the material & pressure/temp loading specs which your have posted above I don't understand those theoretical numbers either.

I've hand-calc'ed (thick & thin) and there is no way you build up those stress numbers either at the middle or ends of the pipe.

What theoretical references do you use??

Sorry if that was not clear.

The total is including contributions for the temperature caused by the temperature gradient as well as the pressure load.

For example, the thermal contributions are around 75 ksi, while the pressure contributions are around 18 ksi. (total of around 93 ksi)

The reason I was using both thick and thin forms of the hoop stress equation was to see how the FEA was interpreting the problem. I believe it is interpreting it as a thin wall problem, when it is actually a thick walled problem.
Not exactly sure how to account for this within the software.

The equation for maximum thermal stress in the tangential direction comes from the Timoshenko reference given by nlgyro

Quote (mtz_engr)

Quote (The reason I was using both thick and thin forms of the hoop stress equation was to see how the FEA was interpreting the problem. I believe it is interpreting it as a thin wall problem, when it is actually a thick walled problem.
Not exactly sure how to account for this within the software.)

You'll have to model your problem as a 3d solid FEM.

Quote (The equation for maximum thermal stress in the tangential direction comes from the Timoshenko reference given by nlgyro)

The peak thermal stress equation is based on a thin-shell assumption. You cannot use is as-is for a thick-shell calc.

Well, I have since modeled it as a 3D Solid.

Pressure only cases match up with expected results from Lame equations for stresses in thick cylinders.

Temperature only cases match up with expected results as well from the equations found in the journal paper below.
Stresses were determined analytically using the Lame equation for pressure and integrating an equation for the thermal stress.
(https://doi.org/10.1016/0020-7403(96)00001-X)

Just an update, to let you guys know I got everything working correctly and to thank you all for the suggestions.

I am now checking how much the results change wrt to mesh density.