I'm trying to generate plots with displacements (T1, T2, T3) relative to a location (node) other than the model origin. Does anyone know if this is possilbe? I thought that the transform output option would do this but apparently not.
Thanks and regards,
Go to View->Options, choose the Postprocessing Category and "Deformed Model" option. Set "Deform Relative To" to "Fixed Node" and choose the Node that you want to deform relative to below in the "Node ID" field.
Or, more simply, go to the Postprocessing Toolbox, choose the Deform category and you should already see a "Deform Relative To" option where you can pick "Fixed Node" and then choose the node you want.
Was not avare of that option. I was however trying to get the contour colors to display the displacements relative to the node.
This macro should help. Here's what it does:
1) select "control nodes": the macro will compute the mean displacement of these nodes and substract it (suppress it) for all nodes.
2) specify outputsets you want to deal with
3) this little hmi pops up:
Now it gets interesting:
3.1) I've dissabled the "include rotation motion". The reason for this is that if you include it, the mean displacement includes rotations and therefore at some point you need to invert a 6x6 matrix. I do this with a 3rd party math library, so it depends on the install...etc...
If FEMAP could include à matrix solver in the API (going only to 6x6 would be enough for a lot of applications), I could pass the entire code.
So anyway check it or not, there's a line in the API that disables it (and the corresponding code is cut out)
3.2) "Apply disp corrections to": so as you say the entire point is to plot relative motion. But if you have a huge model you may not be interested in all of it. So here you can chose on what portion of the model you want to apply the correction.
3.3) "CSys for resutling disp": in many cases I am interesting in the mean displacement which is calculated and corrected. The here will simply allow you to chose in which CSys this will be projected. It changes nothing, only the message written in the window.
This functionnality is something I use all the time, it becomes very useful when you want to understand how something deforms locally, but can't really see it because there is a global "parastic" movement.
PS: oh and it's written for v11.2.1. I think at some point in the FEMAP versions there was a concern with outputs. If you are on v10 there might be a need to reactivate the lines which say "no longer need in FEMAP v11.2"...
Forgot to finish:
4) the macro creates a nodal displacement output vector #9000000 => you can plot it or deform using it
If you've selected a CSys other than 0 for the resulting displacement, it will also create 3 non-vectorial node displacement output (9000010 to 12, X, Y and Z respectively IN THE SPECIFIED CSYS).
Again this goes back to a subtle point in FEMAP: nodal vectorial output is always transformed back to CSys0. Therefore even if you use specific Csys which have "weird" orientations, it's not easy to obtain plots of nodal vectorial output in these CSys. So here this "forces" the creation of these plots in hte right CSys. However it cant' be used as deformed because that would not make sense.
This macro is great. I was performing an analysis on a rail grinder. The grinder consist origionally consisted of 3 cars. The middle car caught on fire and so the customer asked us if we could couple car one and two together. We had to devise a mechanism which preloaded a 76 mm shaft at the center of one car. This pin carried the load of the other car during work or travel and by spec, the entire coupling arrangement was required to carry 1500 kn, a big load. The preload on the shaft was 300 kpf, (I switched units), and there was a weldment arrangement, the bulkhead plate of the machine along with a clevis block, which the 1500 kN load was applied to. All the aforementioned was in the grip of the pin. I wanted to know how much the pin had changed in length and also provide a contour of the relative displacement. Your macro did it. I realize that the program allows you to determine the relative displacement with respect to a fixed node but the contour does not change. Now I have it! Kudos.