SHELL181 and linearization

[beastgod]

Good afternoon, everyone!
sorry for my English in advance.
I use SHELL181 to find stresses, which I must compare with permissible values in according to ASME chapter VIII.
For this I must separate stresses on membrane, bending and peak.
So, questions:
1) Are middle stresses in shell181 equal membrane+peak?
2) Are top/bottom stresses in shell181 equal membrane+bending+peak?
3) when I use SMISC quantities to get numbers from 34 to 47 as in this theme thread569-370754 then my peak stresses are very little even in zone with concentration. Why?

Am I right if linearization in solid elements equal to middle/top/bottom in shell?

Thank you for your answers!

 

[TGS4]

Middle stresses are membrane. Top/bottom stresses are membrane-plus-bending. You cannot obtain membrane-plus-bending-plus-peak from a shell element.

 

[beastgod]

TGS4, thanks for your reply!

so stress concenration doesn`t influence on stresses in shell at all?

Does it mean that when I obtain the top/bottom stresses, I get sum of (Pm+Pl+Pb+Q) and I can compare this sum with Sps?
and consequently when I obtain middle stresses, they equal to sum (Pm+Pl+Pb)?

 

[TGS4]

Although the results from a shell element model can provide you with membrane and membrane+bending stresses, the classification of the stresses thereof depends on the context of the stresses - the location and the nature of the loads generating the stresses.

A couple of notes about stress linearization for the ASME Code. Pm, as general membrane stress, should be a hand calc. The stresses classified as PL and Pb are related to Protection Against Plastic Collapse, and as such are calculated using the design load case combinations in Table 5.3. The stresses classified as Q are related to Protection Against Failure from Cyclic Loading: Ratcheting, and as such are calculated using the operating load range. You should not be considering both stress classifications in the same model.

Also, note that the definition of PL also depends on an extent as defined in 5.2.2.2(b).

I would also highlight the cautions in 5.2.1.2, 5.2.1.3, 5.2.1.4. The use of shell elements is discussed in 5-A.5.3. The location at which the stresses in the shell elements is checked is shown in Figure 5-A.9 and 5-A.10, in addition the general rules and guidance regarding the location of appropriate SCLs should be followed.

 

[beastgod]

Thank you!
I have read chapter V of ASME many times...but to the end did not understand all clearly.
Here I did the simple example to understood better - the nozzle with reinforcing plate and shell. Load is only the pressure.

Can you mark places where I should take stresses each categories?
How can I understand where act influence of concentrator and where not?

seqv middle

http://files.engineering.com/getfil...a-40c5-4efa-af96-d1333ef72846&file=middle.jpg

seqv top/bottom

http://files.engineering.com/getfil...d3-4ed4-bc5b-122c5bb92db3&file=bottom-top.jpg

 

[TGS4]

Are you showing the stress results from one of the Design Load Combinations from Table 5.3, our are you showing the stress range results from one of the operating load ranges?

What are the sizes of the welds attaching the nozzle to the repad and/or shell? How about the repad to shell? How many elements do you have around the circumference of the nozzle? What are the thicknesses of the components?

 

[beastgod]

I have showed the stress results from one of the Design Load Combination - the pressure only (1,5 MPa).
Because we can`t model welds using SHELL181, welds were not modelling.

In attaches there is a picture with [display of element = on] to understand more clearly where is what.

http://files.engineering.com/getfil...74b-4fba-864c-2b2af17b0ee5&file=thickness.jpg

Thickness and sizes-
1) Diameter (inner) of main shell (body) = 3980 mm
2) diameter of nozzle = 480 mm
3) diameter of repad = 800 mm
4) all thicknesses = 20 mm

One more question, if you do not mind:
Noddle or element solution should I evalute?

"How many elements do you have around the circumference of the nozzle?" - Sorry, I didn`t understand this question clearly.

Thanks for your help!

 

[TGS4]

Actually, you can model welds with shell elements - the directions are shown in Fig 5-A.9 and 5-A.10. Furthermore, in determining which location to obtain the stresses from, the direction provided in Figure 5-A.9 has it all there.

Regarding whether to use nodal or elemental values, the simple answer is that the two values should give you the same result, and therefore it shouldn't matter. If the results are different, then your model has too few elements and you need to refine your mesh.

Regarding my question about how many element you have around the circumference of the nozzle - what part is not clear:
a) How many elements...
b) do you have...
c) around the circumference...
d) of the nozzle...

Finally, a comment about your Design Load Combination... There is no load case involving only pressure. You have P+Ps+D as the first load combination. When you refer to Table 5.2, you will notice that D includes a who bunch of tings, including nozzle loads ("static reactions from the weight of attached equipment, such as motors, machinery, other vessels, and piping...").

Finally, regarding your diameters and thicknesses, have you checked the R/T ratio for comparison to 5.2.1.3?

 

[beastgod]

Thanks for helping me, TGS4!
I looked through 5-A.9-10 and had food for thought.
So...in real life I evaluate huge objects as rectification column.

http://files.engineering.com/getfil...0-725e-4e1c-874b-37d43a3e1582&file=column.jpg

1) It must be very small mesh to model welds. But then it takes a lot of time to calculate whole column. so I don`t model welds.
2) I choose dangerous zones, which I will evaluate. Example a nozzle. Then I want to do a sub-model.
3) In solid model (sub-model) I don`t do welds too, because I think it doesn`t influence seriously to stresses in danferous place which located inner.
4) So 'in determining which location to obtain the stresses from, the direction provided in Figure 5-A.9 has it all there' - I should imagine that I have weld, so I should leave 1-2 element from nozzle. There I should evaluate stresses in shell / draw SCL in solid.

I saw one interesting thing, when I was looking the figure 5-A.1. Designers rounded the dangerous place, although in real life it isn`t the same but has sharp edge.(red circle)

http://files.engineering.com/getfil...b2f-4fb9-9900-d5b25c2eea8b&file=2-rounded.jpg

For why they do this, if SCL don`t pass through this point (e.g. fig.5-A.11). and why some figures (e.g. fig 5-A.7) don`t have this rounded point?


"c) around the circumference..." - Perimeter of nozzle? If I right, it has 40 elements.

"You have P+Ps+D as the first load combination." - I understand...but nozzle is blanked-off and hasn`t got any attaches. The influence of weight and Ps tends to zero, so I don`t take them into account.

"have you checked the R/T ratio for comparison to 5.2.1.3?" - of course, my R/T > 4.


Nozzle, which I showed you in previous posts, is only for sample to understand better where I must choose different categories of stresses. How can I understand where act influence of concentrator and where not?

Thanks a lot, I really appreciate your answers!

 

[TGS4]

1) It must be very small mesh to model welds. But then it takes a lot of time to calculate whole column. so I don`t model welds.

It doesn't have to. However, the method shown in Figure 5-A.9 will provide a more realistic stiffness to the nozzle-shell junction.

3) In solid model (sub-model) I don`t do welds too, because I think it doesn`t influence seriously to stresses in danferous place which located inner.

Such an assumption is opposite of what I would do.

4) So 'in determining which location to obtain the stresses from, the direction provided in Figure 5-A.9 has it all there' - I should imagine that I have weld, so I should leave 1-2 element from nozzle. There I should evaluate stresses in shell / draw SCL in solid.

As shown in Figure 5-A.9, the location for evaluation should be at the toe of the weld (whether you model it or not). It would be wise to place a node at that location. Of course, in the process of creating your model to do so, you might as well add in the weld itself - the effort and additional elements (especially for a shell model) is not prohibitive.

I saw one interesting thing, when I was looking the figure 5-A.1. Designers rounded the dangerous place, although in real life it isn`t the same but has sharp edge.(red circle)

http://files.engineering.com/getfile.aspx?folder=f...

For why they do this, if SCL don`t pass through this point (e.g. fig.5-A.11). and why some figures (e.g. fig 5-A.7) don`t have this rounded point?

Sometimes the inside of the nozzle is rounded and sometimes it isn't. Figure 5-A.1 is an illustration of a concept only. Your model may be different.

"c) around the circumference..." - Perimeter of nozzle? If I right, it has 40 elements.

That number of element is, in my opinion, inadequate. I would recommend at least 96 around the circumference/perimeter, as well as an increased mesh density away from the nozzle/shell intersection.

These are some very good questions. Please feel free to return with more. I will note that you are more likely to obtain additional answers if you post your questions that pertain to stress linearization to either forum794 or forum292.

 

[beastgod]

That number of element is, in my opinion, inadequate. I would recommend at least 96 around the circumference/perimeter, as well as an increased mesh density away from the nozzle/shell intersection.

I tested different size of mesh and determined that the most optimal size is 4*t for shell181 (where "t" is thickness).
Here is my work

http://cae-cube.ru/opredelenie-optimalnogo-razmera-konechnogo-elementa.html

I think it will be interesting for you. Sorry, but in Russian only...now I try to explain a little:
1) Fig.1.2 (Рис. 1.2) is the way to analize (Н = start, К = end)
2) Fig.1.8 showed SINT depending on different size of elements from "10*t" to "t" (with a single scale).
3) Fig. 1.9 showed graphs (SINT depend on distance from nozzle). As you can see they same even near the nozzle.
4) Fig 1.10 showed the next graphs.
blue - SINT in MX (scale vertical - MPa, horizontal - size of element)
red - appropriate error regarding the elemnt with size "t"
green - limiting errors (10%)

So, as I can see, reduction of finite element doesn`t significantly affect the stress distribution. So optimal correlation "calculation time-results" is size of element 4*t. I hope it will be useful to know.

Returning to the example in the previous posts, where 40 elements around the circumference, the size of the finite element is 2*t, so I think that's enough. The size of element will be about t, if I do 96 elements around the circumference. For what such accuracy?

By the way, thank you for the timely advices. Now I need a couple days to read some more information and do some tests. And I think I should turn to elastic-plastic analise.
Thanks again, TGS4!