I’m new to ProPoMax and was wondering if there is a way to treat a body of an assembly as rigid (aka not compute stress/strain for these selected bodies)?
I want to analyze the stress in a body that is constrained to a mechanism. For example, a crank slider. If I wanted to do an FEA of the connecting rod but not of the crank or the slider.
I understand that I can be clever with my boundary conditions along with using remote loads, but in my case it would be significantly easier if I could treat the components of the constraining mechanism as rigid bodies.
This would be the same as in Solidworks FEA when you right click a body and select “make Rigid” as opposed to “deformable”. This would save some computing time also.
Sure, you can use the rigid body constraint for that. Just create a reference point in a desired location, then select it for this constraint and specify the region to be treated as rigid. This constraint can be also used to transfer loads (like torque or remote force) to faces.
it seems PrePoMax is not yet completed and needed to add select Element-Set at Region type in menus, currently only possible to assign at node set. However, the solver CalculiX is capable to assign *Rigid body to element set also.
Actually, the *RIGID BODY, ELSET=... definition is equivalent to *RIGID BODY, NSET=... if you select the whole part since internally, only nodes of the elements belonging to the elset, not the elements themselves are used.
But what’s the advantage of being able to use an element set instead of a node set, considering what I wrote above ? It would be useful only when an element set consisted only of a bunch of selected elements of the part. Normally, you select the whole part and then you can just use a node set (or select Part like in the screenshot above).
indeed, select whole surface boundaries is identical also. Only for similarity in feature and interfaces with another FE software, there’s option to convert part to rigid for simplicity,
I see. It could indeed be added in addition to Region type: Selection → Set selection: Part to highlight the fact that the whole part can be made rigid.
rigtht something like these, probably it can be simplified the task. Also, it seems using element set instead of node can be reduced at input files since it’s available by part names.
Thanks for all your responses, sorry I’m still a little confused if we are all talking about the same thing.
FEAnalyst, I’ve tried using the rigid body constraint and it is a great tool as it has reduced by analysis time significantly. However, it seems that it is only useful in situations where you’re imitating a single body only that acts directly onto the body being analyzed, either through force or displacement.
For example, in the attached picture below there are 3 links. The green arrow points to the link for stress analysis while the blue arrow points to the 2 rigid bodies. As I understand it, there is no way to mate a reference point of a link to the reference point of another, which means I cannot connect 1 rigid body to another.
My work around is to treat all 3 links as deformable bodies and make the 2 “rigid” bodies have a very high high Youngs Modulus with a low Poissons Ratio. This works as I have low strain in the 2 links I wish to be rigid. The problem is now I have a long compute time as it’s computing the stresses in all 3 members.
I’ve tried selecting the entire link as a rigid body but the issue is it still requires me to assign a material to the body. If I assign a material and run the simulation it throws an error.
Ideally I would be able to select the entire part body under “create rigid body” but not need to assign a reference point or a material for the body. Then create my surface faces for the surface-to-surface contacts between the 2 rigid links.
It’s not implemented in PrePoMax and thus would require keyword edits but equation MPC constraint should work. It allows you to specify equations between DOFs of selected nodes.
i look the problem sketch and seems to be possible in CCX for all element type (beam, shell and solid). Since there are two member connected share the same common nodes, it is a convenient way using Remove in Equation. Some rotational DOF for beam and shell element model, translation in longitudinal axes for solid element model.
to make a member rigid, it can be simple assign to element set, reference nodes is optional and not mandatory.
is the “m” denotes to mass? if yes, there will be rotational inertia to be considered. Different element type (beam, shell, solid) required specific approach in this regard or simplify by using distributed mass instead of lumped.
lastly, about load scheme in static or dynamic. When static being conducted, make sure all load in equilibrium since the model prone of stability.
I was surprissed about that.
Reading the manual seems it can be read wrong. It is not mandatory that the user define it, but a Rigid body needs a ref node. If not defined by the user, it is assigned to the origin of the global coordinate system by default.
probably there’s many wow on my post please don’t take seriously, just reproduced, test and validates.
when there’s no load or constraint applied to master nodes, is this can make a sense? maybe cause of this, SAP2000 did not require user to defining explicitly.
*edited (add example)
below figure of interesting sample problem from SAP, there’s no extra nodes as master or duplicated nodes with zero length in beam element. Couple will generate internally and automatic by rigid body, no wonder since it’s based on original work of several pioneer and leader in FEA (Clough, Bathe, Wilson)
If the reference node has not been assigned coordinates, ABAQUS will assign it the coordinates of the global origin by default. Alternatively, you can specify that the reference node should be placed at the center of mass of the rigid body.
But the option to apply it to a center of mass is handy.
Has someone try to solve tatertots89 problem?. It seems easy right ?¿?
I’m finding it ridiculous hard to solve.
Is that problem possible with shell elements for example?.
Rigid body shows Stress value?¿?¿, nonlinear fails systematically and dynamic doesn’t allow equation to link the different bodies.
@tatertots89. Do you have some material parameters, dimensions and known solution so we can compare with expected analytical solution??
Regarding using ELSET to define the rigid body on shells doesn’t work for me. That is not new, I have experience that issue a long time ago. It’s supposed to be the same but , doesn’t work for me.
please don’t take seriously, just reproduced, test and validates.