SolidWorks Simulation: FEA of an Heat Exchanger Partition Box ASME VIII-2 DbA

[FPPE]

Good morning,

I need help for a FEA of a partition box inside a channel of an high pressure heat exchanger that I am running for verify the component according to ASME VIII div. 2 Design by Analysis (I attach construction drawings):

Design pressure (tube side): 10.97 MPa
Design temperature: 450°C
Material: ASME SA 240 TP 321

For the material I manually entered its mechanical properties at 450°C.
The simulation was performed with the following loads:

Simulation 1 (External pressure: 0.05 MPa; internal pressure: 0 MPa) ---> max Von Mises 1247 MPa
Simulation 2 (External pressure: 10.97 MPa; internal pressure: 10.92 MPa) ---> max Von Mises 4449 MPa

In the images are shown the trends (I used the symmetry constraint) and the behavior of the first simulation seems to me much more adherent to reality..
The same mesh, constraints and contact conditions were used.
My first question concerns the different results obtained with the same pressure difference between the inside and the outside: can this difference be due to a coarse mesh? The maximum Aspect Ratio is 187; I know that ideally it should be less than 5 to get good results, but I ran the simulation with this mesh just to understand how to refine it later and where. In addition, the maximum values obtained seem to me exaggerated (even if they are present in very small areas.

I would then like to understand how to consider the expansion joint present in the original drawing and understand why this was used. The displacement at that point (lower part of the partition box) is on the order of 0.2 mm. Do I have to consider the pressure thrust or I consider it automatically absorbed by the joint (otherwise why was it inserted?)?
I have not inserted any force due to pressure thrust in these simulations.

Thank you for your help.

 

[MJCronin]

WOW... very exotic.....Massive thickness on the channel end !!! (Is that all thick 321 SS???)

Is this not a First Extraction Feedwater Heater for a thermal powerplant .... perhaps a Nuclear Plant ????

What is the tubeside fluid bulk modulus and will it expand if it is trapped within the HX ?

Wild guess here, but could the tubeside EJ be protecting the shell against tube rupture if the tubeside fluid expands ?

(Again, I am guessing here)

MJCronin
Sr. Process Engineer

 

[TGS4]

Please forgive me, but this post is very confusing. Let's start by working through ASME Section VIII, Division 2, Part 5 - what Failure Mode are you starting with? If you are working with Protection Against Plastic Collapse, then what method are you using: Elastic, Limit Load, or Elastic-Plastic? From there, which load case combination are you evaluating? You indicated some peak stress values - but what about the values of P[sub]m[/sub], P[sub]L[/sub], and P[sub]b[/sub]? How have you validated your model (what hand-calcs have you done?)?

 

[FPPE]

Please forgive me, but this post is very confusing. Let's start by working through ASME Section VIII, Division 2, Part 5 - what Failure Mode are you starting with? If you are working with Protection Against Plastic Collapse, then what method are you using: Elastic, Limit Load, or Elastic-Plastic? From there, which load case combination are you evaluating? You indicated some peak stress values - but what about the values of Pm, PL, and Pb? How have you validated your model (what hand-calcs have you done?)?

Of course you're right. I'm working with Protection Against Plastic Collapse with an elastic analysis.

Following the linearization of the stresses in the section shown below (for the simulation with only 0.5 bar external pressure), I obtained the following values of the membrane and bending stresses:

The allowable material stress at 450°C is 116 MPa (to compare the membrane stress). S_pl is equal to 1.5*116=174 MPa (for membrane+bending comparison). The stress peaks result at the bolted connections, probably the bolts are undersized or I need to modify the preload (imposed equal to 9046 lbf axial for a bolt in SA 193 B8T, AISI 321, 1/2").

So:

Membrane stress Pm (0.87 MPa) < Allowable S (116 MPa) ---> OK
Pm+Pb (point 1) < S_pl ---> OK
Pm+Pb (point 2) < S_pl ---> OK

Obviously I have to make this check in more sections (especially near the tubesheet and in the flanged areas).

WOW... very exotic.....Massive thickness on the channel end !!! (Is that all thick 321 SS???)

Is this not a First Extraction Feedwater Heater for a thermal powerplant .... perhaps a Nuclear Plant ????

What is the tubeside fluid bulk modulus and will it expand if it is trapped within the HX ?

Wild guess here, but could the tubeside EJ be protecting the shell against tube rupture if the tubeside fluid expands ?

Hi MJCronin, no only the partition box is in 321 SS. I do not know this information. So you think the joint is only needed in an emergency?

For Protection Against Local Failure, where can I find in SolidWorks Simulation the three principal stresses to compare with 4*S (parag. 5.3 of ASME VIII div. 2 - triaxial stress limit)?

According to you, in theory, do the results obtained seem compatible with reality?

 

[NRP99]

-Why are you doing analysis? For 0.05MPa you do not need to do analysis which can be seen from the results (Pm<1MPa). Simple hand calculation to check the plate thickness is sufficient.
- Flat plates will not sustain high value out of plane pressures. That is why all pressure vessels are "round" and that is why the partition plate is exposed to very minor pressure.
-For local failure, you need to combine three principal stresses S1+S2+S3 and check for all nodes/integrations points for S1+S2+S3<=4S. You need some sort of user defined results(combining results or input of equation) facility to input above equation. Check whether that is available in Solidworks. Check=>Results Equations in solidworks help.
-I am unable to understand why you are getting peak stresses in range of 1000MPa. This may indicate wrong constraints or wrong loading values or worst, element quality is really poor. Thoroughly check your model from senior engineer/mentor/experienced analyst.
-Are you using linear tets? Try quadratic tets. Use refined mesh in the areas of the discontinuities. If possible do a mesh convergence study. Verify the model with just a simple load first.
-I will suggest to read and solve problems from ASME PTB-3 to get some basic information before diving into project assignments.

 

[FPPE]

Why are you doing analysis? For 0.05MPa you do not need to do analysis which can be seen from the results (Pm<1MPa). Simple hand calculation to check the plate thickness is sufficient.

Thank you for your response.
The analysis was requested by the client.
I used a preload on the bolts equal to 40000 N. The gasket is made of KLINGERSIL 400 BLACK GRAPHITE. How should I calculate the correct preload (axial or torque)?
The Bolts are in A193 Grade B8T for high temperature and high pressure service.
Thank you

 

[Lolloo]

For Simulation 1 (External pressure: 0.05 MPa; internal pressure: 0 MPa) ---> max Von Mises 1247 MPa
i think you should have used "buckling" module of Solidworks Simulation to find eigenvalue, von mises in linear analysis makes no sense.

 

[FPPE]

i think you should have used "buckling" module of Solidworks Simulation to find eigenvalue, von mises in linear analysis makes no sense.

I used "static" module. Could you explain what differences the "buckling" module would lead to in this specific application? Thank you.

 

[IdanPV]

"Simulation 1 (External pressure: 0.05 MPa; internal pressure: 0 MPa) ---> max Von Mises 1247 MPa
Simulation 2 (External pressure: 10.97 MPa; internal pressure: 10.92 MPa) ---> max Von Mises 4449 MPa"

Can you share pictures of those locations showing the mesh?

 

[Lolloo]

If the external pressure is present, the buckling shall be considered.
You should referer:
ASME VIII Div 2 5.4 Protection Against Collapse From Buckling
ASME PTB-3 2013 Example E5.4 – Protection Against Collapse from Buckling

 

[Lolloo]

The linear "buckling module" is part of the Solidworks Simulation Professional package.
Non-linear buckling analysis can be performed with the Solidworks Simulation Premium package.

 

[FPPE]

Can you share pictures of those locations showing the mesh?

Hi IdanPV, I attach pictures below:

I modified the mesh until I got the properties shown above. I still think the problem may be the bolts.

If the external pressure is present, the buckling shall be considered.
You should referer:
ASME VIII Div 2 5.4 Protection Against Collapse From Buckling
ASME PTB-3 2013 Example E5.4 – Protection Against Collapse from Buckling

If I select the buckling analysis in the "Component interactions" tab it only gives me these possibilities:

- Bonded
- Free

I would need to use a contact without penetration as in the case of the static analysis. Do you know if there is another way? Thank you

P.S.: I set the maximum stress value in the legend equal to 174 MPa, but as shown in the first pictures the values in the bolt area are much higher. I know they have no real physical sense since the material plasticizes first, but still I would like to be clear if there is a problem in the simulation setup.

 

[IdanPV]

Hello,

The higher stress at the bolts area may be "artificial" without any physical meaning.
I suggest you to run non-linear static analysis just to check those area.
Moreover, you may want to check the ERROR plot at this area, a 5% error is a good benchmark to see if the results can be used.

Take a look at this articles:

https://www.pveng.com/stress-classification-lines-scl-passing-through-areas-of-very-high-error-post/

https://www.pveng.com/error-plots-bolt-heads-and-surface-to-surface-contacts-post/

Source: PVEng.com

 

[FPPE]

The higher stress at the bolts area may be "artificial" without any physical meaning.
I suggest you to run non-linear static analysis just to check those area.
Moreover, you may want to check the ERROR plot at this area, a 5% error is a good benchmark to see if the results can be used.

Thank you IvanPV, I I found these articles very helpful.