Press Fit Simulation in Optistruct
Altair EmployeeDear All,
I want to do press fit simulation of two cylinders with interference of 0.6 radially by using NLSTAT in Optistruct.
can any one please guide how to do it.
Regards,
Suraj
Answers
-
PFA sample deck for Optistruct solver on pressfit simulation.
0 -
Hello,
sorry to come back to a problem that has already been addressed in the past, however I am having some trouble validating the results from your example to an excel that I've made a few years ago in order to calculate pressure and stresses due to interference fit. I made runs both on the file contained in your PCONT.zip and the files contained in the File.zip from the following thread:
Based on your model I measured the following diameters: Inner tube radius: 5.010 (dia = 10.020). Outer tube inner bore: 4.999 (dia 9.998), outside radius: 7.974 (dia = 15.948). Thus the interference fit is: 10.020 - 9.998 = 0.022 (diametrically). I trust that these values are all in mm since in your example you have used MPa as the E value for your material. I am working on inches, psi units in my excel, so I had to convert the above into inches (divide mm with 25.4) and check what the excel gives. Your FEM gives for the contact pressure a value of 878.707 MPa wheras the excel calculation... well you can see for yourself the large difference. Any ideas? (note: 1psi = 0.00689 MPa). In addition: although both models in your examples, have the same dimensions, the different use of MORIENT selected value (NORM in one case, OVERLAP in the other), has a substantial impact on the results (with NORM, the calculated pressure is: 1910 MPa). Please note that my excel calcs have been verified with worked examples.
Thank you.
<?xml version="1.0" encoding="UTF-8"?>
<?xml version="1.0" encoding="UTF-8"?>
<?xml version="1.0" encoding="UTF-8"?>
0 -
Hi @mvass
Could you please share the excel sheet using the file transfer link which is available in my signature below?
0 -
Hi Pagadala, thanks for your reply.
I cannot transfer the excel file that I've made at the moment. Please find attached two pages with the calculation (you only have to perform the calc for the contact pressure (pc) on the first page. I am truly sorry for the inconvenience.
Regards,
mvass
edit:
this result seams much closer (stress, pressure):
<?xml version="1.0" encoding="UTF-8"?>
0 -
hi, did you try to calculate the contact pressure? I'll try to upload the excel file today. Is the stress, pressure result that I've shown above the correct answer? Or should the contact pressure be what we are looking for?
Thanks.
0 -
0
-
I've calculated as per the doc and I see the pressure at contact surface is approx 140MPa
I will check and update you soon.
0 -
Altair Forum User said:
I've calculated as per the doc and I see the pressure at contact surface is approx 140MPa
I will check and update you soon.
Thank you very much for taking the time to repeat the calculation. As you saw, contact pressure is about 140 MPa (137,34 MPa as per my excel). The question now is, how to relate this to the optistruct solution. As seen from my previous post, only the pressure calculated from the stress options is close to the value obtained from the FEM solution...
Please have a look, I think many people will be interested in this sample problem.
0 -
Hello again,
please find attached my latest working example of a press fit analysis. Despite my efforts, I couldn't make it show the contact pressure results in hyperview. Please let me know what I did wrong and I'll let you know the outcome of my analysis after that.
Thank you.
0 -
0
-
Hello,
I still cannot find out how to visualize the 'contact pressure' in my model (although I have included the contf option in the results), but I'll share my calculation results with you:
The model I've created is in inches-psi and the dimensions are taken from the excel used for performing the analytical calculation for an interference fit case. It has been verified with an example from the book that contained that exact calculation. As to the optistruct model the solution is a NL quasi static, with an auto-contact between the two components (surface-to-surface if I am not wrong) created using the respective utility. One note here: the creation of a contact between all the overlapping elements, leads to a .fem file that takes a loooot of time to converge even with my coarse mesh of model elements. The contact group MORIENT flag was set to 'OVERLAP' and the NL analysis was submitted to the solver. Results:
1) The solution predicts a displacement (magnitude) of the outer component contact diameter of 0.00132 inches (diametrically = 0.00132 x 2 = 0.00264 inches) which is very close to the 0.0028 interference fit set for the calculation.
2) As said before, I could not have an option for the 'contact pressure' so I visualized the results for stress pressure. As seen, the calculated results from the analytical calculation are 5000 psi and 3000 psi for the inner and outer contact surfaces respectively. The FEM solution predicts values of 5673 psi for the inner contact surface and 3515 psi for the outer contact surface. Again, I am not sure if my approach to read the stress, pressures is correct (see previous question).
Thank you for your time.
<?xml version="1.0" encoding="UTF-8"?>
<?xml version="1.0" encoding="UTF-8"?>
<?xml version="1.0" encoding="UTF-8"?>
0 -
Hi Mvass,
Did you use CONTF>> PCONT?
This should output contact pressure. It would be great if you share the model and results.
0 -
Hello and thank you for your reply.
Of course I've used CONTF-->PCONT as you can see in the .fem file that I've posted a few days ago. Since I have not access to HM right now, please run the .fem file attached in my previous post and check the results. I as said before I cannot find 'contact pressure' option in HW (although I have used the PCONT option) and I would like to know if my assumption about stress,pressure results is a correct substitute.
Previous message (with the .fem file) follows:
Altair Forum User said:Hello again,
please find attached my latest working example of a press fit analysis. Despite my efforts, I couldn't make it show the contact pressure results in hyperview. Please let me know what I did wrong and I'll let you know the outcome of my analysis after that.
Thank you.
Thank you for your interest.
<?xml version="1.0" encoding="UTF-8"?>
0 -
Hi @mvass
I see that the contact pressure at surface is way far from close compared to stress.
I am going to discuss with experts and I will get back to you soon.
0 -
Hi @mvass
Here are some suggestions from our experts:
CLEARANCE option on CONTACT card can be used to do interference fit modeling, which is better than simply relying on geometrical penetration based on mesh coordinates.
There are also two issues in the boundary conditions of this model. Firstly, the inner ring is not well constrained and it can rotate along its axis arbitrarily since the contact is frictionless. And secondly, the constrains (the two circles of SPCs) at the outer ring will make its deformation be drum-shaped instead of log-shaped. Here are two approaches which you may ask the user to consider for a better model setup:
1) Set the boundary conditions in a cylindrical coordinate system if the two rings share the same axis. Fix the rotation of the rings and fix their axial translation at their one ends.
2) Use a 1/8 section of the full model and fix the three planes of symmetry.
0 -
hello & happy new year!
I am sorry that I didn't see your reply earlier. Thank you for your effort. I'll try to follow your suggestion for a new model & BC setup and when I'll have the results I'll post them here for further discussion.
Best regards.
0
