I have encountered the following several problems when studying NozzlePro Software:
（1）：There are 3D shell element and 3D brick element in the NozzlePro。When we do the stress analysis of the thin wall Pressure vessel,we ususlly choose the 3d shell element.In my mind,we can only get the membrane stress and bending stress(Pl+Pb+Q),and can’t get the peak stress in this model.
In asme VIII division 2, the peak stress with 3d shell element model can be calculated using this formula（as the picture）

There are two facts in the nozzlepro with 3d shell element model:
a)the Pl +PB +Q +F also be analysized to meet with SA limit in the nozzlepro with 3d shell element model
b)using the Pl +PB +Q +F to calcalculate the sif in the nozzlepro with 3d shell element model
so ,how do you get the F,or how do you get the Kf when doing these analysis?
I think just only the 3d brick model can be used to do it exactly.
2)Pl+Pb+Q< 3Samvg,why don’t you use 1.5(Sc+Sh) ,but use 2Sy for 3Samvg?
3)Pl +PB +Q +F < Sa, why the value of Sa is neither the values of "B31" Fatigue Stress Allowable or the value of Markl Fatigue Stress Allowable

Maybe you should address this question to the software developers, PRG (Paulin research Group) in Houston.

Section VIII Div 2 provides FSRFs to get between membrane and bending stresses and the fatigue life of the component. You will find those in Tables 5.11 and 5.12 of VIII-2 Part 5. For as-welded geometries, the peak stress cannot be readily calculated using brick models either, due to the singularity at the weld toe. In this case the membrane+bending stresses are found by integrating thru the thickness of the geometry, to get the M+B stress. In this case the same FSRFs are used to get from the Pl+Pb+Q stress (secondary) to the Pl+Pb+Q+F stress (peak). The method has been effectively validated for carbon and stainless steel geometries and weld quality. Caution should likely be exercised when there are high cyclic loads in materials not as thoroughly tested, or when new welding procedures are being used.

There are concerns that elastic approaches (brick, shell or axisymmetric) for primary loading may be overly conservative in certain pressure optimized situations, i.e. where Pl+Pb
Paulin Research Group
NozzlePRO Tech Support

Hello,Paulin’s technical egnieer:
I have encountered some another problems when studying NozzlePro Software:
1) If there is only a same pressure load at the cycliner and branch intersection.if I use the inside diameter to calculate the longitudinal pressure thrust(P*A),I see the softwarte automatically to provide two directional forces of FX,FY.
I think The Fy is for the Run cycliner longitudinal pressure thrust,and the Fx is the difference of the Branch longitudinal pressure thrust by using mean diameters and using inside diameters.
My question is that: the applied location of theses two forces are different ,one is at the end of Run cycliner,the other is at the end of Branch, the software provide these two forces in the same case in the reports, do the software automatically apply these two forces in different run and branch boudanary?
2)as mentioned above,the NozzlePro automatically add two logitudianl forces to calculate the local stress at the junction discontinuity due to pressure in the longtitudinal, but how to calculate the the local stress at the junction discontinuity due to pressure in the circumferential.
This will influence the local stress at the inside corner.
3)why the NozzlePro Provide the same normal stress due pressure (PD/2t) at both run and branch?

Here is the response form PRG:

Question 1:
I think The Fy is for the Run cycliner longitudinal pressure thrust, and the Fx is the difference of the Branch longitudinal pressure thrust by using mean diameters and using inside diameters. My question is that: the applied location of theses two forces are different ,one is at the end of Run cycliner, the other is at the end of Branch, the software provide these two forces in the same case in the reports, do the software automatically apply these two forces in different run and branch boundary?

Answer:
The forces printed are the summed unbalanced loads from the finite element model for each load case, and as such reflect the unbalanced pressure thrust that acts on the model and is reacted by the boundary conditions. The loads act over the appropriate finite element surfaces and are compiled in the global X,Y and Z coordinates for convenience. They are provided to be used just as you have used them, to validate that an appropriate overall load is applied to the model.

Question 2:
2)as mentioned above, the NozzlePro automatically add two longitudinal forces to calculate the local stress at the junction discontinuity due to pressure in the longitudinal, but how to calculate the local stress at the junction discontinuity due to pressure in the circumferential.
This will influence the local stress at the inside corner

Answer:
NozzlePRO does not add to individual “forces” per se, but rather provides a pressure load from an integration over the surfaces of the model exposed to pressure. Since pressure applies everywhere on the id of most geometries, the pressure loads will produce stresses at critical inside corners in longitudinal planes, (where pressure stresses in branch connections are usually highest), but also throughout the remainder of the geometry albeit at usually lower magnitudes.

Question 3:
3)why the NozzlePro Provide the same normal stress due pressure (PD/2t) at both run and branch?

Answer:
Any dimensionless parameter that’s a multiplier on the pressure could have been used. PD/2T is the nominal pressure stress used historically in VIII-2 calculations and so NozzlePRO used the same for consistency. The piping codes B31 use pd/4t as the nominal pressure stress in the respective branch and run pipes, where VIII-2 uses the properties of the vessel (run) only. The selection is arbitrary as long as the use is consistent.

Thank you very much for your reply
1)As you mentionded,NozzlePro doesn’t add individual “forces” but rahter provides a pressure load from an integration aver the surfaces of the model exposed to pressure.
I also think this is the right method.
But if NozzlePro uses the integration method ,the pressure load on the surface will be self-balanced ,I only understand that ,when I set the” Options” to use mean diameter ,the Fx will disappear, Why does the Fy force exist in the report? why doesn’t the FY force be self-balanced by the two run ends?
2) AS you mentionde ,PD /2t is the nominal pressure stress used historically in VIII-2.what I concern is that :
a)whether the magnitude by “PD/2T” be considered as a global membrane stress to be addde to the total stress?
b) on the contraty, does the magnitude by “PD/2T” only be calculated in order to meet with VIII-2. Does the total stress be not directly associated with this magnitude.the nozzlepro get the total stress by the equilibrium equation from the finite element model?
above what i said is to assume there is only a pressure load in the analysis