flange joint, two probs, one question

iii

Dear Victor,

at the first, you created great software, easy to work with it, etc. But I need help with two little problems. I am ansys user, some years experience with fem/fea analysis. Our task is often to analyse flange joint. Usually flange joint with complicate thermal fields, non linear gasket, many load cases, fatigue etc etc. So my model is often only section with one bolt, for example 1/24 etc.. I want something similar create in your Mecway. Nowadays I am only "free user", so I am limited to 1000 Nodes (this is great possibility to try your soft), which is enough for test case (Fig1). My problems (model imported from step files):

1) nodes with contact cant have also displacement constraint (for symmetry). (Fig2) I can solve this problem with merging nodes of flange and gasket, and then apply symmetry. Or selecting other nodes for contact and others for constraint. Have you something more elegant?

2) I created bolt with beam element (I like this solution). It is possible to create some multiple MPC contact, or joint -> to direct connect 1 node (beam) with whole surface under nut? CE (constraint equations) for each node pair is time consuming, for 6 DOF and at about 20 node pairs (for one node pair Fig3).

3) adding bolt pretension will be great feature (for me, of course there are other possibilities how to solve this problem)

For better illustration I also attach some figures. I use shell for flange only due node restriction (and quick coarse ).
Thanks, best regards, Igor

ps: please, do you have also something like verification manual for Mecway (for licensed user)?

Victor

Hello iii

1) There isn't an elegant solution. Your second suggestion is probably the most general. One way to do that is by extruding a thin layer of elements out from the edges. Then you can use the newly extruded nodes for the symmetry constraints and the original nodes for contact. Being a thin layer, it can cause an arbitrarily small error in the solution.

Another way is to use elastic support for the symmetry constraints instead of displacement or frictionless supports. With this method, you'll have to choose a stiffness high enough to prevent deformation by not so high that it introduces numerical error or fails to solve.

2) You could use bonded contact here. Model the head of the bolt as solids which only needs a very coarse mesh with a central node connected to the beam. Then make that the master surface for bonding with the flange.

3) I'm aware of ANSYS's bolt pretension for cylindrical surfaces but don't really understand what it's doing. Are you looking for something different from the spring with preloading that Mecway has? Perhaps one where you specify the preload as a force rather than a displacement, or one that works with solid elements? A workaround for solids is to use thermal stress as preload.

Verification. Most of the samples in the manual are also verifications with the results being compared to hand calculations. I find that most people want to verify very different situations so it's difficult to create a broad enough set of cases.

This is a bit naughty, but you can reuse some of Abaqus's verification cases since it can import many of those files. I just tried one (ecs3sfs1.inp) which successfully solved and gave the same stress solutions shown in the Abaqus Verification Manual section "1.3.1 Membrane loading of plane stress, plane strain, membrane, and shell elements". The file and description are here http://www.egr.msu.edu/software/abaqus/Documentation/docs/v6.7/books/ver/default.htm?startat=ch01s03abv04.html