5 Replies Latest reply on Dec 11, 2013 8:45 AM by Bill McEachern

    FEA Divergent Result Issue - ASME / API Flange Design

    Shawn Guillory

      Hi,

       

      I am looking to find someone whom is an expert in SolidWorks Simulation FEA to possibly help me out with this problem I am trying to solve.

       

      To provide some background on what I am doing and the issue I am facing:

       

      I am working on preparing engineering design packages according to API 6A Specification for 5,000, 10,000, and 15,000 psi flanges of various sizes.  The mating faces are slightly different when you get to pressures of 10,000 psi and above and thus have a raised face rather than just a flat face.  However, running the FEA should be the same setup for both styles and only the hand calculations are somewhat different due to the lower pressure flat face flanges having a standoff (gap) between the flanges upon makeup vs. the raised faces being made up until they virtually touch.

       

      Below are snapshots to give you an idea of this:

       

      SolidWorks Submission 1.png

      3D Assembly of Raised Face Flange without Bolts, Exploded View, and Section View of Exploded View

       

      SolidWorks Submission 2.png

       

      API 10,000 psi (Raised Face) Flange Prior to Bolt Makeup: Gap Between Flanges = 1/8 inches

      Note: BX Style Gasket is Somewhat Oversized by .046 inch to Provide a Pressure Energized Seal Upon Bolt Makeup

       

      SolidWorks Submission 3.png

       

      API 10,000 psi (Raised Face) Flange After Bolt Makeup: Gap = 3/64 inches

      (Not Full Makeup Which Occurs After Pressuring Up Which Results in No Gap)

      Note: The stresses are quite high and you can see where the potential problem with the thin inner lip bending outward and into the bore area of the flange

       

      SolidWorks Submission 4.png

      API 5,000 psi (Flat Face) Flange to ASME Code Design Prior to Bolt Makeup: Gap Between Flanges = 1/4 inches

      RX Style Gasket is On Center with Groove and the Inner Lip is Much Thicker so it is Expected to Not Cause As Much of Problem. However, since there is a large Gap that remains even after bolt makeup, the bending moments on the flange will be much higher which are largely absorbed by the bolts.

       

      SolidWorks Submission 5.png

      API 5,000 psi (Flat Face) Flange to ASME Code Design After Bolt Makeup: Gap = Slightly Less than 1/4 inches (Not Much Change Which is Expected and is the Way These are Designed)

       

      Note: The stresses are quite close to within reason except for some hot spots and you can see where the thicker material of the thin inner lip keeps the inner lip from bending outward and into the bore area of the flange. Overall, this looks like a good design despite that the hot spots in very small area of material are exceeding the yield stress limits (So, mesh refinement might yield more realistic results which hopefully put it within acceptable limits).  However, and upon subsequent mesh refinements, the stress keeps going up and up indefinitely which is surprising as I expected it to be about like this in magnitude…but in refining the mesh to the radii to eliminate the unrealistic high stress spots and thus lower the maximum stresses to within under the minimum yield strength of the material at 75,000 psi and on the order of under .83% of the yield strength at 62,000 psi, the results just diverge instead of converge to a limit.

       

      In preparing these design packages using hand calculations, I am following the ASME Section VIII code for flange design.  The stresses calculated by this method are coming out within reason for both style of face for the flanges.  However, and being somewhat concerned that the code calculations due to St. Venant’s Principle and thus the code style hand calculations not considering the local stresses caused by the pressure energized gasket meshing into the groove of the flange, I decided to run SolidWorks Simulation FEA Static Analysis on the full assembly.  However, and in running the FEA, I have been unsuccessful in converging to the result.  The FEA will run, and the gasket will compress into the flange groove and seat into that groove like what it does in reality (which seems like this will provide a good result), but the results do not converge regardless of applying fillets to internal sharp corners and applying what seems to me to be reasonable mesh controls putting the element size at least 2 widths on those faces of concern.  The stresses are certainly coming out too high by the FEA method for safely passing along with diverging and appear to cause concern on the inner lip of the groove that is near the bore of the flange which is what I was actually concerned about it doing since:

       

      1. The ring gasket gets compressed .046 inches in overall diameter shrinkage for the raised face flanges with BX style gaskets…which isn’t going to cause much load and thus stress and potential damage to the flange if the gasket were made out of rubber but this gasket is pretty thick and it is made out of stainless steel.  Imagine compressing a steel ring inward on how difficult that would be and how much force it will in turn tend to press back.  That is what is happening when the flanges are bolted up together with this BX style ring gasket between the two flanges.

       

      2. The ring groove on the raised face flange is very close to the inner bore thus resulting in a thin lip and thus due to the resulting force from the compression of the ring gasket, it may indeed cause the inner bore lip to bulge inward and into the bore which will lead to loss of the sealing effect needed.

       

      3. I researched and discovered that a team of flange design engineers with one of the top major oil & gas corporations ran FEA with ANSYS showing excessive stresses from high pressure flanges all the way through the entire cross section on the ring gasket thus enacting a change in the gasket in the coming years.

       

      4. API, the American Petroleum Institute, hired an engineering consulting firm out of Houston to perform FEA on flanges to come up with a specification called API 6AF1 & F2 if I remember correctly (may be named slightly different) to develop charts of limitations on the flanges along with external loadings.  However, the manner in which the FEA was simulated uses assumptions of a line load being placed on the ring groove rather than actually using the gasket which does not and cannot possibly simulate the effects of the actual ring gasket compressing into the ring groove.  I have also seen many other firms utilize the same methods for analyzing flanges which of course would never show the resulting stresses actually occurring in that region, which is a region of very high interest since it provides the seal, and that in turn brings up cause for concern.

       

      5. Lastly, API has a situation for the 6A spec which states that of all of the wellhead equipment that is designed to 6A, if a company’s 6A license has the phrase “NO Exclusions” then they have to provide design packages for every product licensed and sold under 6A.  However, if the license has the phrase “Exclusions Apply” or something to that effect, then of all the “standard” items licensed and sold under 6A, which flanges are so standardized that they have charts of all the dimensions for all of them including the gaskets, ONLY the flanges require design packages and none of the other products require design packages.  This sends the signal to me that regardless of the flanges being standardized, API currently wants design engineers to still analyze only these flanges more for sure out of all of the other products under this specification, and that certainly is more than likely for a reason which some sort of failure with these high pressure flanges is the only reason that I can ascertain.  To mention, ASME flanges were pressures from under 1000 psi to I believe up to 3000 psi and were much heavier and bulkier.  But API flanges are more optimized in the design putting them with much less material and smaller bolts which I believe is due to the pressure energized gasket design which allows the flanges to make up virtually face-to-face rather than being separated by a rather large gap.  This allows the bolt load to be carried by the flange faces which in turn (according to someone’s theory) result in the gasket width being independent of the bolt load and thus the lip between the groove and bore can be somewhat narrower than in the ASME code design since it does not carry any load (but there may be some issues in real life with this thinner lip possibly proving this theory to be not as accurate and with the tools of FEA today we can hopefully show these stresses and deformations better to show that this is where the problem is).  You can see the difference between the ASME code style design heavier flanges with larger inner lip vs. the API design style flanges with a much thinner inner lip in the picture below.

       

      SolidWorks Submission 6.png

      Smaller Lip API Raised Face Flange Design vs. Larger Lip ASME Flat Face Code Design

      Picture Above Taken From Design of High-Pressure Integral and Welding Neck Flanges with Pressure-Energized Ring Joint Gaskets, 1964, R. Eichenberg

       

      To provide a little data on the 10,000 psi Raised Face Ring Type Joint Flange:

       

      Standard 2 9/16" Flange - Dimensions as per API 6A (75,000 psi Yield Strength Alloy Steel)

      Gasket - BX-153 as per API 6A Standard Dimensions (Stainless Steel)

       

      I am simply applying a fixed restraint on the bottom extended piping portion of the bottom flange to keep the assembly in place while not resulting in tampering with the results in the portion of interest and applying bolt type connections of about 30,000 lbf of axial loading to each of the 8 - 7/8 inch bolts to simulate just bolt make-up load and tightening the bolts and thus 2 mating flanges to a gap of about 3/64 inch based on the code design of 50% of the yield strength of the bolts and the actual cross sectional area at the root of the bolts.  Then proceeding with two ways of testing this:

       

      1. With a shrink fit analysis since the gasket is oversized by .046 inch (However, and since the faces actually mate up, although off center and to one side, this can really be simulated with No Penetration Contact Sets between the 4 mating faces that make up the corners of the ring gasket with the 4 mating faces of the walls of the groove on the flange itself)

       

      2.  With No Penetration Contact Sets between the 4 mating faces that make up the corners of the ring gasket with the 4 mating faces of the walls of the groove on the flange itself

       

       

      Both methods worked in providing similar results of showing the gasket actually compressed into the groove with a final gap of approximately 3/64 inch but both with similar divergent stress and deformations between resulting mesh set runs.

       

      To provide some background on the mesh and process along with snapshots:

       

      I started out with a global course mesh of .75 inch only.   Automatic transition was not used since the mesh fails using this option at this high of global mesh.  Also in trying the automatic transition, I noticed it did not provide the mesh refinement in the areas necessary and needed so I stayed clear of this.

       

      Then I decreased the mesh in half to .375 inches which provides a pretty good balance of element size without being too large or too small for the overall assembly model and also gives me a good method of checking for convergence due to halving of each subsequent run.  However, the external radius of the flange was only one element across the face of this as well as in the area of the flange ring groove and also only one element across on the gasket itself in all areas… the elements were mostly only one size across in these areas of concern and my understanding is that this needs to be at least 2 across for minimalistic good results.  There are also internal sharp corners in the groove itself but they have small radii on each corner of 1/32” which should hopefully prevent the infinite divergent stress situation of the FEA mathematical model being based on the theory of elasticity which will result in infinite stress the finer the mesh in areas of internal sharp corners.

       

      Moving along, I then reduced the global mesh to .1875” which helped out in the areas of the external flange radius as well as on the ring gasket and flange ring groove putting 2 elements across on most areas.  However, it provided unnecessary amount of elements for the overall flange thus increasing calculation time tremendously.  Nonetheless, I needed to attempt to see the convergence without any false assumptions being taken, so I did not use symmetry or load simulating gasket action or anything of the sort and just ran the FEA on this despite the large number of elements to process.

       

      Nonetheless, and through the 3 smaller mesh sizes, neither the stress nor the displacement converged.  I then added mesh controls to the small fillets in the ring groove and other portions of the groove as well as on the ring gasket which produced even more elements to process and ran that.  The results still did not converge and appear to produce different results every time I have ran through the process of redoing all of this multiple times.

       

      Below are snapshots of the final mesh with mesh controls:

       

      SolidWorks Submission 7.png

      Global Mesh Size = 0.75 inches (Poor Quality Mesh Results – One Element Size Across the External Radius and One Element Thick Across the Ring Groove Features as well as the Gasket Itself)

       

      SolidWorks Submission 8.png

      Global Mesh Size = .375 Inches (Pretty Good Mesh Overall on the Assembly Model with 2 Elements Across the External Radius and on the External Portion of the Raised Face…However, There Needs to be Some Refinement Still in the Groove Area and the Gasket Itself)

       

      SolidWorks Submission 9.png

      Global Mesh Size = .1875 Inches (Improvement in the Groove and on the Gasket But at a Sacrifice to More than Necessary for the Overall Assembly Model in Other Areas…However, it Still Needs Refinement to the Groove Depth, Inner Raised Face Lip and Internal Radii of the Groove as well as the Angled Flats on the Gasket Itself that Actually Mate within the Groove)

       

       

      SolidWorks Submission 10.png

      Global Mesh Size = .1875 Inches along with Mesh Controls of Various Sizes to Specific Needed Areas which Resulting in the Above Mesh.  Looks to Me to be Like a Pretty Good Mesh for Getting Good Results That One Can Rely On…However, and with More Refinements, the Stresses and Displacements Do Not Converge

       

      Furthermore, I have looked into p and h-adaptive methods and they were unsuitable.  The p-adaptive was certainly unsuitable and the h-adaptive did refine the mesh in the right areas upon successive loops but did not refine the fillets enough nor other areas enough.  Regardless, and in checking the Convergence graph of the adaptive methods, the stresses and displacements clearly diverged instead of converged.

       

      I have also looked at Direct Sparse vs. FFE methods but was really I found to be unnecessary to do so.

       

      I have run these studies over and over again and as Einstein was said, doing the same thing over and over again and expecting different results is the definition of insanity (I know you heard that one a thousand times).  In any case, I am an engineer so I am probably already insane, but I am hoping someone can help me out and put some level of sanity back into this mix and possibly provide some insight into what I may be overlooking or doing wrong or explain something about the intricacies of the FEA program and what is necessary to trick it and yet still provide suitable results.

       

      Thanks much in advance for anyone’s input on this.

       

      With Kind Regards,

       

      Shawn

       

      P.S. Below is a picture of the dimensions for the raised face flange if you can make out the flange lines vs. the dimensions (you probably can) in case anyone wishes to kill some time and try this out themselves. Note that some dimensions are not necessary to recreate the flange and are only part of the API hand calculation analysis for moment arms of the forces used in the calculation and other dimensions for calculation purposes rather than needed to recreate the flange. The picture is the left side half of the flange...you can see the 1 inch bolt hole on the left side just to orient you to this picture with the center line to the right side of it:

       

      SolidWorks Submission 11.png

       

      If you wish the check the hand calculations to see that they are within reason, you can use ASME Section VIII Div 3 Part 3 in conjunction with an article explaining the design of this newer method that one can purchase online from ASME by the name of:

       

      Design of High-Pressure Integral and Welding Neck Flanges with Pressure-Energized Ring Joint Gaskets, 1964, R. Eichenberg

        • Re: FEA Divergent Result Issue - ASME / API Flange Design
          Jared Conway

          is the TL:DR version of this that you aren't getting convergence of BOTH stress and displacement?

           

          displacement is where you should be spending your time and if the above is correct, post your model or if you're looking for some more direct support/training on this, feel free to contact me at jared@hawkridgesys.com and we can find a way to help you out with this.

          • Re: FEA Divergent Result Issue - ASME / API Flange Design
            Mike Pogue

            First, I'd like to nominate this for question-of-the-year, 2013.

             

            Some thoughts and questions:

            • If this is a code flange, is it necessary to provide analysis?
            • What is the goal of the analysis? To show that the bolts won't break the flange when tightened?
            • In general, you will see divergent calculated stress where the contact conditions change discontinuously. What you should see is, as you decrease the element size around the discontinuity, you can concentrate and shrink the divergent volume around the discontinuity. Stress far from the discontinuity will converge ("Far from" just means "however far you have to go to see convergence". This will get closer and closer as you reduce element size). At the same time, strain energy for the entire part, even including the divergent volumes, will converge. You can continue this process until
              • a.) you feel like the volume showing in yield is structurally insignificant, and the mathematically convergent volumes have the correct safety factor (good), or
              • b.) you feel like a mathematically convergent section in yield is going to cause the part to fail (bad)
            • Finally, though I'm not familiar with code high pressure flanges, this looks like a compression fitting, which depends on local yielding for correct function. A linear analysis cannot give you accurate stress values in the yielded areas.
            • Re: FEA Divergent Result Issue - ASME / API Flange Design
              Bill McEachern

              Hi Shawn,

              Nice post, though I am not sure what/where exactly is not "converging". Given my cursory inspection of the post and fogive me if I haven't studied it up in sufficient detail. However here are my thoughts. I would think that you are unlikely to get a "good" answer here with a linear analysis with good being defined as stresses and displacements limited to a sensible range of values. I get from your text that it is expected that all the results are to be sub yield and so the thinking goes that a non-linear analysis is not required. I would disagree with that as a blanket statement, until it has been proven to be so. The successful operation of the of the actual gasket likely depends on plastic or at least non-linear deformations, which when they occur lower the peak response to the gasket it terms of stress. Further the use of bolt connectors, an idealization,  would also result in the stresses around the bolt holes to be unreliable. They typically over predict the stresses in the surrounding material, at least in my expereince. The successful resolution of your conundrum would be an iterative approach to figure out what subtleties would need to be included to resolve the stress regime to your satisfaction if you wanted to work with me on this. I can be reached at billmce@redstone6.com. I have some expereince working on ASME Section VIII div 2 vessels.

              It has been my expereicne that a non-linear analysis will resolve issues such as these due the fact that a non-linear solution will required convergence iterations and tends to relieve or bleed out peaks in stresses. Further you may want to look at the element stresses as opposed to the nodally averaged stresses and see how they vary over the various meshes you have tried.

              Good luck with your investigation you are probably lined up to learn a lot about how this stuff works if you pursue this to its resolution.