i want so simulate the displacement of a plate which is connected to four bended rails.
is use the 101 linear static solution with default parameters in "case control" -> "global contact parameters"
the fem model looks like:
the plate has fixed constraints on four polygon faces on his bottom side.
the rails are fixed in horizontal direction (Z & X) and have a 0D Mesh with element properties "CBUSH (Grounded)" and 0.01 N/mm in Y translation so its statically determined.
I used "face to face contact" and no loads. My thought was that due to the contact between rails and plate, the rails will be straightened and the thick plate will be slightly bent.
but the result was:
the rails were bent INTO the plate
how can i avoid this? I tried different settings, but always the same result..
Solved! Go to Solution.
Without the NX AdvSim model in hand, what I see is that you have defined only ONE connector between the plate & four rails. This is not correct, you need to define FOUR connectors, one for each rail.
When defining Contact Regions the user should avoid to have islands of elements, all contact elements should be continuous, not possible to include in the same region the four isolated rails, OK?.
i tried it now with four seperate connectors for each rail
all with the same settings.. and the result was
one rail was bent in opposide direction.... dunno why
there was just one warning: "NUMBER OF OUTER LOOP ITERATIONS EXCEEDED"
du you need the files or any futher information?
Yes please, zip all your files of the NX study (*.prt, *.sim, & *.fem) and I will take a look t it, anything is wrong defined.
Regarding the message "iterations exceeded" you have reached the default maximum contact iterations of 20, simply in the global contact parameters of the BCTPARM nastran card increase the number to say 35, but if in 20 contact iterations the contact solution do not converge then it seems to have a problem.
Your NX AdvSim simulation confused me, I don't understand the aim of the calculation: you don't have defined any loading, neither a contact interference, neither a gravity load. The solution monitor show how the LINEAR contact solution progress, but I have my concerns, I will explain later:
By the way, I have REVERSED the four connectors, TARGET region should be the plate, and SOURCE region the rail, this is where the contact elements are created, so the reduced area and more flexible body should be choosed always as SOURCE.
Here you are the results, use SCALE DEFORMED SHAPE 1:1, if not everything will be scaled 10% of model size by default giving a distorted image of reality (Edit POST VIEW and click in DEFORMATION). But in any case the results are useless, this is a LINEAR CONTACT analysis (SOL101) where small displacements is the assumption, and you have parts with gaps more than 30 mm, this is useless at all, results are nothing, simply colors. To properly perform a contact analysis using the assumption of small displacements of linear contact the components would be touching each other, with ZERO gap distance, if not the solution should be treated as minimum as NON LINEAR by the geometry, activating the LARGE DISPLACEMENT effect, OK?.
Also, try to use CHEXA elements when possible, you will reduce the model element size a lot , will speed analysis and increase accuracy of the results, compared with tetrahedral CTETRA elements.
thank you for your efforts!
you don't have defined any loading, neither a contact interference, neither a gravity load
do I need a load? The rail is bent and should have contact with his complete surface to the plate.. because of this there are forces applied to both parts without any external forces
The displacement of the rails can be much lower (about 1/2 mm) this was just for testing (i didnt know that this causes problems in linear statics).
I tried it a second time just with one rail and the plate as "target". Furthermore I used the 0D Mesh PBUSH in XYZ for the rail so its only "fixed" because of the surface to surface contact.
My problem is that there is still no contact between rail and plate at the Ends (just in the middle). Is it possible that this is just wrong displayed?
When i hide the rail and amplify the deformation I get a reult as expected
You can solve a contact problem without external loads, of course, this is the case of “Snap-Fit“, “Press-Fit“, “Interference-Fit“, “Overlapping“, etc.. problems (take a look to my blog in the following address: https://iberisa.wordpress.com/2012/01/16/tratado-c
Probably (I don't know, I am guessing) you want to know the force to apply to rails to have fully contact with the plate??. In this case, a procedure could be to prescribe an enforced displacement at the tip of the rails, but in any case this should be solved as NONLINEAR because you have an important GAP distance between bodies, and because you have surface-to-surface contact then you need to use the ADVANCED NONLINEAR module (SOL601) because the basic nonlinear module (SOL106) only support CGAP elements, understood?.
Alternatively, instead to prescribe an enforced displacement at the tip of the rails, you can apply a load to the rails and graph the resultant displacements, or the extension of contact in the plate, this way you can see the relation between applied load & contact pressure, etc..
I think I understand your problem: you believe that defining a "surface-to-surface contact" is like forcing to both bodies to be in contact for sure??. No, this is not the case, CONTACT is not an enforced displacement boundary condition: you are defining a NO PENETRATION contact, where both bodies can deformed according applied loads & constraints & material properties, but the contact condition simply prevent penetration between both bodies, do not enforce anything!!.
Surface-to-surface contact conditions allow the solution to search and detect when a pair of element faces come into contact. The contact conditions prevent the faces from penetrating and allow finite sliding with optional friction effects. The surface-to-surface contact source and target regions consist of shell and/or solid element faces. From element faces in the source region, a top and bottom normal is projected. The software creates a contact element if:
Any of the source element normals intersect with an element in the target region.
The distance between the two faces is equal to or less than the defined separation distance.