Nodal force & displacement output on selected surfaces from a global model

[vugru]

Hello,

Is it possible to output the "resultant forces" on a few selected surfaces from a large global model that has been already solved? I have multiple "load sets" in this global model and want to write the resultant forces for all these load sets. The idea here is to create a "break out model" with more accurate geometry and finer mesh details and drive this model using the nodal forces at the boundary surfaces obtained from the global model.

[346gnu]

Vinnie,

The answer is yes and no. In your case possibly more no than yes.

General background, Simulate, né Mechanica, solves the mathematical problem and uses this solution to calculate the values (stresses, strains etc) at the grid points and stores these in the results files.

The solution is then thrown away. (very frustrating and would probably solve your problem)

You are left with files with lots of numbers. You then us the post processor to delve into these files and produce pretty pictures.

This goes all the way back to RASNA and computers with limited resources. Only ask for what you have space to store.

So for measures (eg, constraint reactions, directional contact forces, stress errors etc), if you don't ask before you run a study, the software will not calculate and store them.

Always ask for more measures than you need. If you forget to ask for them they can often be inferred by considering equilibrium and free body diagrams. In other words, you can reverse engineer the values quite a lot of the time.

However, you refer to loadsets and resultant (not reaction) forces.

Firstly there is a Review Total Load function which permits you to calculate (about a csys) the components of a number of forces you have applied. (You cannot use this function to include the effects of inertial forces, you have to add contributions from inertial forces in by hand calc).

Secondly, in the rpt file (summary or run status file) the resultant loads acting on the model are reported for each loadset. These resultant loads DO include inertial forces.

Your 'break out model'. You allude to sub-modelling. It is possible to create bonded/contact interface measures to report the forces/moments. This works for volume regions too. But what you really need is the nodal displacements at the interface and this can't be done.

Additionally, if you were to use the forces, you don't know the nodal distribution of those forces so your break out model would have to be much larger and you then have to trust that StVenant was right. The 'sub model' would have to be in static equilibrium and you would use the 3 point constraint method to hold it.

It is possible to build the model and define displacement measures at many points on a boundary of an area to be modelled in more detail. You then apply these movements as enforced displacement constraints in your breakout model at each of the points. The method works but is tremendously tedious and error prone and a few blind alleys. There is no automation to help you and your nomenclature needs to be tight. Subsequent geometrical changes (what ifs) are likely to mess things up.

So back to the global model without fancy methodology. Keep the mesh as basic as possible over the whole model such the global model is as lightweight as possible. What we want is the area of interest to be in the middle of something with the correct surrounding stiffness. Use mesh refinement on your local area only. At the moment, this is the best way.

Sometimes you just have to have a big model. However, connections and geometry a long way from the area of interest should be simplified.

Always ask for too many measures, in particular component measures for interfaces and constraints.

Much more to say but ought to do some work

bfn

[vugru]

Charles,

Thank you for your response. I have tried creatng measures in the "global model" on the "surfaces" which would be the boundary of the breakout model for "force resultants", Fx, Fy, Fz in my model with all solid elements. I only get one value for each boundary surface, for each force resultant. What I need are the force resultants at all the grid points (preferably), or at least at the end nodes of the element faces lying on the boundary surface. I'm using the default grid points of 4. The only way I know is to use "brute force", i.e., break up the boundary surfaces into several tiny surfaces and then create measures for each corner of these smaller surfaces. Further, the breakout model needs to have the same features on the boundary surfaces. This whole process is not practical.

Another issue with Simulate with very large assembly models is that it is a battle to get the AutoGem to mesh the model. With fine "regular mesh" that is needed for further analysis in the local regions of interest, it has become next to impossible to get the global model to mesh. It would be so helpful if there is a way to acquire the resultant forces either through simple measures created before the solve, or, from the post processor. Hope PTC folks are listeing and come up with a solution.

Enough said... getting back to work.

[346gnu]

There is no silver bullet.

For a bonded connection you can create fx fy fz mx my mz.

Though this will not help you with your quest for nodal forces (or forces at grid points). If heading down this route I would measure displacements at user defined points rather than forces and apply enforced displacement constraints.

But as I said earlier, this is tedious and error prone. (and I have a nagging feeling that hard points do not work inside a volume,,, I will experiment on Monday)

You should re-evaluate your need to create this sub model and re-evaluate the need to have a large assembly. Simplify the structure away from the area of interest to keep the elements to a minimum.

There are good strategies for meshing models with many components. (There are some other threads here somewhere) It is a learned skill. You will never see a nice hex-dominant mesh and don't assume that other software is without its foibles and necessary simplifications etc. Other software is just a different 'black bag' of tricks... even if they do support sub modelling.

Sometimes you need to run the study several times. Each run has the refinements in a different location. This would be the nearest practical method of 'sub modelling'. This is the approach I use first.

Unfortunately we have had to have very large assemblies in Simulate all at once. There was not a time saving way around things. We would not have got the correct estimates for deflections of the overall structure if we had bonded all the fastener connections. However, once we had the deflections of the global structure we could apply enforced displacement constraints to subassemblies using the component interfaces.

A way around having the full model in session is to carry out studies of sub assys to estimate their stiffnesses. Then build a simple 'equivalent' stiffness model using general beam sections and springs. This method works well but you can see the amount of preparatory work required before you build up back to a top level model and you need a rock solid modelling strategy.

A study type becomes really difficult when the mass distribution is changed by simplifications is anything with an acceleration, modal and vibration will be affected.

Can you give more info about your model?

Consider how the a380 wing rib designers get their loads.

For the PTC folks you mention, I would put sub-modelling ahead of RAM as an enhancement. I have, for sometime, been meaning to comment on a thread I read somewhere. Sub-modelling would mean less RAM required. Having more RAM whilst always welcome does not mean better models.

Thanks