I'm new with Femap I'm a just graduated mechanical engineer, I am trying to obtain the stress profile in a contact between a cylinder and a convex ring of a bearing.
The goal is try to plot the stress profile for varoius convexity.
The models seems well biulted, but I find very boring to export data in excel for every model to build a graph with multiple data from multiple model.
My question is: is there a way to plot different model results in one graph in Femap? Or maybe is it possible to have all the geometry (for different convexity) and the analysis in one model in order to have all the result data in the same graph?
Thanks for the help.
Assuming the changes in convexity are "quite small", you could use one model and one mesh to analyse all the cases. The way to do this is to create multiple surfaces representing the different convex ring surfaces, and then adjust the model by projecting the original convex surface nodes onto the new surfaces. The command is Modify -> Project -> Node. Note that you can select the nodes using Method -> On Surface and select the surface(s) that represent the original convex ring. You then choose the new surface to project the nodes onto. Note that the nodes remain associated with the original surface even though you move the nodes off that surface. Thus for each new case of convexity, you still use the original surface as the method to select the nodes to project.
Similarly, even though you probably used geometry to define the contact (is this Linear Static iterative linear contact or Advanced NL Static?), the contact is calcuated based on the location of the nodes and element faces, not the geometry itself. This means you do not need to redefine the contact regions even though the nodes will have moved off the original surface.
In this way, you will be able to run each convexity case using the same mesh but with the nodes moved slightly to represent each case. Your model will end up with multiple output sets which are all associated with one consistent mesh, and your Femap charts will update easily if you use the All Output Sets option.
As this is a contact analysis which requires extreme precision to get quality results, your mesh should be reasonably fine and "neat" (ie an orderly mesh pattern on the faces, not a "free mesh" style). Also, if you are making very precise changes in the convexity, I suggest you also use "Large Field" format for the Nastran analysis file, via Model -> Analysis... expand your Analysis Set, expand the Options, click on Bulk Data and press the Edit button. Choose Large Field.
Finally, if you are doing this contact using non-linear analysis but with gaps, then a different technique is required, because the gap opening is a property of the gap and not a function of how far apart its nodes are.
Very helpful! thank you for your explaination and patience.
Tomorrow I'll try this technique, if you have time could you please help me in other problems with my model? I'll explain better: the analysis is linear static, the geometry is a part of the revolutioned ring (only 30° to minimize elements) with a simmetry constraint, in the same way the cylinder, witch has all fixed surfaces. I wasn't able to better simplify the geometry, I have tried to mesh only the top surface of the cilynder (plate elementes) but it gives me wrong results.
For the stress profile I convert the stress vector (max values) on the nodes and plot the value on the curve in contact with the cylinder, but also with relativly small mesh, it gives me the right trend, but the result for near nodes are oscillating, Could it be a problem of mesh sizing? I've tried to modify the mesh but sometimes it fails and sometimes the model is too complex for my machine.
I hope you or someone could help me, if it's necessary i'll try to upload screenshots or other files.I'm really new with fem and i can't wait to lear because i really like using it!
Oscillating contact result is probably related to precision or refinement of the mesh. I forgot to explain that is the reason for choosing "Large Field" format. Femap still must write a text file for calculation by NX Nastran. The standard "field size" is 8 characters which is not enough for precision contact. Eg this Femap node coordinate -0.0023455001 would be written as "-2.346-3" in the NX Nastran file. Precision of only 4 significant figures is not enough for good contact stresses in metals. Large Field format creates field sizes of 16 characters (double precision) which is plenty for accurate contact stresses. Femap itself operates in double precision all the time.
The model needs to be huge (eg. >500,000 nodes for simple contact on a medium computer) or the computer quite basic for the model to be too complex. If you are a new user, the main reason why models fail to run is usually some error with the modelling. Femap and NX Nastran are very robust, but FEA has many tricks and traps!
Sorry for the late, i've updated the model with your suggestions, now i'm trying to optimize the number of elements vs time and memory used. I haven't try the node projection jet, I can't really understand how to draw the surfaces where to project the nodes, but for now i'm focus on the single result.
For a better explaination of the oscillating results I've uploded a screen of the graph of the Von Mises Stress vs the axial quote, we can see that the differences between the max values for differents radius is very small and because of the oxillation, I can't really see the behaviour in the centre of the ring. Will a more precise mesh reduces this error? Thanks a lot!
It's a little hard to guess without seeing the mesh, but if you want the best quality contact result, then it is best if the mesh is "matched". That means the pattern and quantity of nodes on one contact surface should match the pattern and quantity of nodes on the other contact surface. Thus the nodes should be fully paired across the contact interface (but do not accidentally merge them). The mesh should be regularly spaced, or if you have refined the mesh in the contact zone, then the refinement should be progressive and tidy on both interfaces as you move towards the zone of highest contact pressure. You should also create / select a group of nodes which is a direct track across (one of the) the contact surface that you will use to plot the output. If each of your plot lines represented a single track across the contact surface, then you have more than enough mesh (looks like hundreds of data points per curve). If it is not a single track (eg just stress vs position for the whole surface), then the noise may simply come from the noise in "coordinate position" versus where that coordinate is located on the surface.
Lastly, you need to be sure about what result you are plotting. Stresses typically belong to elements and corners of elements. Node results are displacements, constraint forces and some contact forces. If you have not been thorough (eg. if you have not deliberately converted element corner stresses into averaged nodal stresses via Model -> Output -> Process), you possily have plotted the element centroidal stress vs position - which is the easiest default choice to have made when requesting stress vs position results. Element centroidal stress results are very likely to be noisy, because the depth of the centroid below the contact surface will be quite random - unless you have the most perfectly controlled mesh style across and along and through the geometry you have meshed.