Reaction Summation on Fixed Support

cwharpe

Hello. New to Mecway. Really impressed.

Looking for a quicker way to sum the nodal reactions individually selected fixed supports. I've been copying to clipboard from the Solution Table and then pasting into Excel, but I was hoping there was a more direct method.

Also, I can't seem to find the csv file that I am supposedly writing when I Solve. Is this just me?

~CWharPE

cwharpe

Update: CSV File written in the same directory as the current Mecway model. Was looking in the wrong place.

Still wouldn't mind an on-screen summary, though.

Victor

Hello cwharpe

Yes, same directory as the model, unless you specify a rooted path like C:\...

Unfortunately, there currently isn't an easier way to sum the forces but I agree it'll be a useful feature.

Sergio

Hi, in Abaqus I can do this summatory, but sometimes is easier to setup a rigid body between one master node and all the rest nodes of the fixed side, so then is just to ask for the reaction in this master node. Is possible to do this in Mecway? Maybe using truss elements?

Regards

Victor

That's an idea. Here's an example using bonded contact to transmit the forces from a large number of nodes to a smaller number, then beams to transmit them to a single fixed node that gives a reaction moment and force for the whole surface.

You could skip the bonded contact and only use beams but that would get tedious to create all the beams if there are lot of nodes on the surface. Alternatively, you could skip the beams and just constrain 3 nodes of the rigid element to give 3 reaction forces that you can use to manually calculate moments from.

Victor

Picture of model in previous message.

Sergio

Is possible to define a named selection of nodes (what I interpret as a group of nodes) with the slaves nodes and then use it to add a RIGID BODY definition as a custom model definition for solving in Calculix?

I have tried, but the node set and rigid body definition is writted in the inp file but ccx refuse to solve (attached lml file).

Best regards

Victor

Yes, this model is set up the way I would expect. However CCX seems to have the same limitation as Mecway in not allowing constraints on MPC slave nodes. I tried to work around it by extruding a thin layer on the SLAVE_NODES surface so they're not the same nodes as have the adjacent constraints. I also changed the reference node from 4 to the newly extruded one. Not sure if I've retained your intended meaning or not because the solution is a bit funny.

Sergio

And what about define a named selection of nodes and then in the table results filter by this selection of nodes using CCX? I can do it using Mecway solver but when I switch to CCX I loose that (usefull) possibility.

Regards

By the way, I have solved (file included) with CCX and then try with Mecway and have very different results, do you have any idea?

Sergio

file from last comment

Victor

Thanks for the suggestion about node selections through CCX. It's not entirely trivial because CCX sometimes changes the numbering but I'll see how it goes.

That file doesn't solve correctly with the Mecway solver because of the non-zero displacement which isn't supported.

Sergio

Thanks, otherwise getting the nodal summatory is hard even with Excell. I has to take note of every node in the fixed side and then filter by hand for every iteration of the solution step in order to get the load/deflection curve.

Tim_Gowing

Hi Victor, Sergio,
I'm looking for an efficient method of creating an MPC within Mecway for CCX. I am interested in both the kinematic coupling ('Nastran-RBE2' type MPC, stiffness added) and the distributing coupling ('Nastran-RBE3', weighted average displacement type MPC, no added stiffness). I have typically created the distributing coupling in CCX using a *EQUATION statement, where the sum of the displacement of the independent nodes is equal to the displacement of the single dependent node. Three of these statements are required when dealing with 3d elements, for x,y & z dofs. This can also be achieved by using the CCX *distributing coupling.
The tool that I am looking for in Mecway allows me to:
1) choose between creating a) kinematic coupling and b) distributing coupling
2) choose an existing 'Node_Selection' for the independent group of (multiple) nodes
3) choose an existing 'Node_Selection' for the dependent (single) node
4) choose the degree of freedom for the constraint, individual x,y or z, or a combination such as x,y & z.
5) write out MPC(s) for desired dofs a) *Rigid Body & *RIGID BODY,REF NODE=nodenr (kinematic, RBE2) or b) *DISTRIBUTING COUPLING & *ELEMENT,TYPE=DCOUP3D (distributing, weighted average, RBE3)
In the example image below, the created MPC would look like the spokes of a bicycle wheel, between the blue nodes within the bore to the central red node.
I believe that the bonded contact functionality already writes *EQUATION statements for the nodes belonging to a set of element faces; the MPC here requires a single node rather than the second surface.
Can the manual create constraint equation method be used for CCX to create the weighted average constraint (multiple independent nodes & single dependent node in one statement)?
Tim

Victor

Hi Tim

I hope to do something like that for future versions, but probably not v5. A few people have asked for it.

Can you please clarify point 4) What are the use cases for using only some of the DOFs? Can that be satisfied by connecting the single node to the rest of the model through a truss element/spring/equation instead?

Currently, you can make a *RIGID BODY by entering the CCX cards manually under CCX -> Custom model definition. I expect you can do *DISTRIBUTED COUPLING the same way too.

Including the Constraint equations in Mecway for exporting to CCX is another thing for a a future version. For now, you can use them with Mecway's solver to get a connection with one node having the average displacement of a set of nodes. It would just need one big equation for each of the 3 displacement DOFs.

Please start new threads for new topics. That can help people find it because the title will match the content better.

Tim_Gowing

Hi Victor,
Thank you for considering the further CCX MPC creation tools.
The selection of dofs in 4) replicates the tools in Patran and the like, I will typically use all three translation directions, dofs x,y & z. The situation where you may only wish for say 2 dofs would be where a component is supported via a bolt hole in each of three lugs; the 'distributing' MPC is selected at each of these bolt holes to avoid artificial local stiffening and allow a reasonably accurate representation of the load path within the lug. The bolt hole axis may all lie in, say, the x-y plane. Now it is not possible to constrain the single dependent node of the coupling (*EQUATION) as an error will result (application of a force is ok), therefore the workaround is to create another node coincident with the single dependent node and connect these with linear springs of great stiffness such as 1e9N/mm, in the applicable dofs. The three component lugs may constrain particular dofs in order to not over constrain the component overall, i.e. lug1 constraint on x,y,z, lug2 y,z and lug3 z. The SPC would be applied to the node on the stiff spring.
Back to the question, when using the CCX *DISTRIBUTED COUPLING then x,y and z dofs are connected, between node group and single node. When creating this MPC using *EQUATION then there is no need to create a constraint equation in a dof that will not be used, i.e. lug2 x-direction.
I suppose I favour the *EQUATION method for creation of the weighted average displacement MPC (RBE3), even though the *DISTRIBUTED COUPLING is specifically provided for this purpose (old dog, new tricks).
Tim

Victor

I see.