Welcome to MCAD Central

Join our MCAD Central community forums, the largest resource for MCAD (Mechanical Computer-Aided Design) professionals, including files, forums, jobs, articles, calendar, and more.

Register Log in

Analysis of a Vase of Pressure

amd450

New member
I'm beginning in this area, i think that my problem is with constraints but ratio of error is very high, approximetely 15%, and the example is apparently simple, the inlet pressure is 5,1 N/mm
 

Luis Aguirre

New member
Andre,



What is the error ? Is the error in displacement, stress, etc ? how did you compare your answer ? from lab data hand calculations ? I will check your file and see if I can see any problem but It will be helpful if you can answer my other questions.



Luis,
 

amd450

New member
I did like shell, when I ran the file appear a message accusing a error between shells, but I didnt find gaps or something that can be a error. (in my opinion)
 

Luis Aguirre

New member
Hello Andre,



Well I had a chance to take a look at your file. So far I had found two possible problems. One with shell compressing as you mentioned and one with modeling.



Shell compression (problem #1): The shell compression is failing because you hace two types of thickness in your model. The upper part is made of thinner material tha the bottom part right were the two different thickness meet mechanica creates a gap because is trying to compress the to intersecting shells at the mid-plane. The solution to this problem is to compress the planes to the face (inside wall) that both share the same location. You can do this by using the edit shell location and shoosing the inside wall and click on the adjencent option so all the rest of the shell will automatically have their midplane move to the new location. When you are readu to run the model mechanica will warn you about the shells not being compress to the mid-plane. Accept the warning and let it run.



Symmetrical assumtion ( Problem #2): The geometry for most of the part may be symmetrical, however; the constrain condition appears not to be radially symmetrical. However, I assume there are another two points of attachment besides the one showing in the symmetrical mode? If that is the case then your symmetrical assumption is correct. But your symmetrical constrains are not. You are using a cartesian coordinate system when you should be using a cylindrical coordinate system to set up the symmetry constrains. To solve this problem create a cylindrical coordinate system in having as center the axis of symmetry of the model. The create new constrains (remember to use the inside edge for their location) change the coordinates system from the default to the cylindrical coordinates. Set the displacement Z and Radial coordinates free and let the tangetial coordinate fix. For the rotation do the opposite.



I have the student version of wildfire at home so I don't think my model will be of much help since you are using 2001. However, when I go back to work next Monday I'll see if I can fix the model there and send you a working copy. Feliz a~o nuevo.



Luis
 

amd450

New member
Thanks Luis for your answer, I did what you said me, I inserted news coordenates (cylindrical), I saw that the upper thick isnt inffluencing in the final result, so I put constant thickness. The error not appear, but there are 11 elements that didnt convergence and the Local Disp is 26,3% and the Global RMS was 20,2%. Do you think that this here isnt higher? I'll attach the file.



Thanks other time.

PS.:Obrigado e Feliz ano novo para voce tambem



Andr
 

bem

New member
Andre:



Check your symmetry constraints again. For displacements R & Z should be fixed and theta should be free. Just the opposite for rotations.



I changed the symmetry in your model and got it to converge. Summary file attached. Under the analysis menu for multi pass adaptive change the maximum polynomial order to 9



There appears to be something funny happening in the z displacement. I would check your model for buckling. I will try to look at it if I have time
 

Luis Aguirre

New member
Andre,



Your boundary constraints are not set properly as bem mentioned. However, I think bem ment to set the R and Z free and theta fixed. The way, you can check if you have the correct symmetrical contrains is by imagining the cutting plane that created the symmetry and see if it can move freely in those degree of freedom without crossing in to the material. For example, in this case your cutting plane is the R-Z plane. If I move the cutting plane in the R-diretion or up and down (Z-direction ) the cutting plane does not overlap the material. However if you move the plane in the theta direction then it will cross into the material. Therefore, when you set your constrains the R and Z directions must be set to free so to allow the material to move in that direction and theta must be fixed to prevent the material from overlaping into itself. You can do the same exercise for the rotation but at the end you will realize that the rotation constrains are set opposite to that of the displacement. This is done because the displacement, strain, and stress field must obey the compatibility equation which asures that the field (FEA mesh) does not create a case where the material will overlap itself.



I have include the model with the proper constrains. I get a convergence of 3% in maximum/minum stress using Single Pass Adaptive (SPA). I did not try to run it using Multi Pass Adaptive (MPA). But the results should be very comparable unless you have a singularity in the model.



Luis



P.S. Andre how were you able to upload your zip file? I was not able to do it myself. Apparently there is a size limitation of 50 Kb per file. But your zip file is 145 kb. Is there a trick to upload a file of this size. Let me know so then I can post the model file .
 

bem

New member
Whoops! Sorry about that. I mis-typed, Luis is correct. I meant to say R&Z free, theta fixed. Attached is the file (2001).



Now that we have that settled, I am a little concerned about the inclusion of both pressure & mass. If this vessel is pressurized, I guess that's ok. But if the pressure is caused by the material inside, it might be more appropriate to create an non-uniform pressure distribution (i.e. p= density *g* height)



Has anyone done this? (storage tanks, silos etc)



ps Luis - I think the size limit is on embedded picture files, not zipped attachments
 

amd450

New member
Thanks for everybody. (Bem) Sorry I mistaked, this equipment is a Silo and inside have Sugar. Like I'm beginning now in this area of Analysis if I mistaked please correct me in relation about forces, reaction etc. (Luis Aguirre) I sended a blank file and after appear the option to attach a file or edit. Any sugestion more are welcome.



Andre
 

Luis Aguirre

New member
Andre,



The bottom surface that contains the bolt holes must be fixed as well on the normal direction. I think is your y direction otherwise the bolts holes are supporting all the weight.





Luis
 

amd450

New member
I did any changes, my boss dont wanted that I did cut in the part, like I sended to homepage before, I put the constraints in the holes where will be bolted (only this) where will be supported, I did 2 analisys Pressure and Force, the inlet pressure is 0,5 bar and the force (weight of sugar) is 166 ton, and there are a force in case of explosion of 320KN in the support. How I express the weight of sugar in the volume? Normally whitch is the ratio of error accetable (GLOBAL RMS and LOCAL), when for example there are 1000 elements and 2 dont converged, in this case what do I do? I sended again the file.



Thanks everybody.



Andre Almeida
 

Sponsor

Top