Solid Von Mises Stress results visibility issue

[Anonymous]

Hi everyone!

I don't know why the results of the Solid Von Mises Stress in the Fatigue Analysis don't appear. I'm talking about the coloured bar in which results are shown. The only thing I can see is the Plot and results of the Solid-Life Countour, but I am also interested in knowing the static results such as the displacement, deformed, von mises and safety factor, which are the ones that I can't see.

(The results are wrong because they are so high. If anyone know why it would happen please tell me.) These are the results I am able to see, but the ones that I am not able to see are the following:

Also, I'm not able to generate a report of the results. 

Thank you very much in advance.

[John_Holtz]

Hi @Anonymous 

The fatigue results are wrong because you are using version 2019 and have multiple loads applied. See Multi-axial fatigue analysis with multiple loads not displaying multiple results in Nastran.

I do not know why the stress results are not shown. Is it possible that one of the applied loads gives results of 0? A stress of 0 would give infinite life which is what 1E10 shown in the fatigue life is indicating. I believe that version 2019 does not show the legend bar if all of the results are the same value, such as 0.

• For example, is one of the load applied at the same location as the constraint?
• Is there a displacement result? If you display the deformed shape and contour the displacements, the min and max displacement will appear in the legend (if it is shown) and in the text at the bottom of the window (where it shows what result is displayed).
• Were there any warnings in the analysis?

Otherwise, if you can zip your assembly files (.iam) and part files (.ipt) and attach it to the forum, someone will take a look at your model.

[Anonymous]

Oh yes. I think one problem could be that, I will install the 2020 version.

And also, yes, the loads are applied in the same spot than the constraints, but that in this case (connecting rod) I can't think about other spot to place them. No displacement is shown in my analysis and also  I have two kinds of warnings: the warning E5085 and G3012, but I don't know exactly what they mean.

I will upload the files just in case anybody could help me.

Thank you very much!

[John_Holtz]

Thanks for the model @Anonymous 

The problem is that ALL of the loads are applied at the same locations as the constraints. So the loads go directly into the constraints and create a reaction force; none of the load goes into creating displacement and stresses. 

With the stresses being 0, the part has an infinite life. I think it is over designed. 😄

I assume the large bore is "fixed" to the crankshaft. Therefore, the large bore should be fully fixed. No loads need to be applied to the large bore because there are no external loads on the part at that location. (The reaction forces from the constraints create the "load" that occurs at that location.)

The small bore is attached to the cylinder. The small bore is allowed to deform in all directions relative to the large bore, except for maybe in the Z direction. (It depends on the construction.) Assuming no constraints on the small bore would certainly be a conservative approach. The small bore is certainly not constrained in the X and Y directions which are the directions of the applied loads.

Let us know how your new analysis turns out.

[Anonymous]

Wow, thank you very much, I didn't think of it in that way. And also sorry for the late reply.

I just got the Fatigue results, thank you very much again, you've helped me so much!!!!!😀😊 I'm uploading the picture with the results. I also changed my version to Nastran 2020.

But I have one final question... Is there any way in which I could see the results in each point/node of the piece? 

[John_Holtz]

I am glad you are making progress.

For your last question (see the results at each node), you should clarify exactly what you want. For example, there are probably 150 different results (or more!) available, 3 different subcases (2 sets of stress results and 1 set of fatigue results), and 100000 nodes or elements (maybe more). Do you really want a list of 150*3*100000 = 45E6 results? I hope not! But if that is what you want, you can edit the analysis ("Analysis > Edit") and change the Output Options from "Plot" to "Print". The output file will include a printout of all results, all subcases, all nodes and elements. (Hint: The result on line 5,985,478 is wrong 😁.)

Usually, 1 type of result for 1 subcase at very specific locations are of interest. Some options (from easiest to more complex) are as follows:

• Right-click on "Nodes" in the model tree and choose "Query Display". Hold the mouse over nodes of interest.
• Click "Results > Probes" in the ribbon. hold the mouse over areas of interest. Note that the probe interpolates the results between the nodes, so it is difficult to repeat an exact reading since it does not "snap" to a node.
• If you have 10 or fewer points, you can create an XY Plot and select multiple items. When you show the plot, you can copy the data to the clipboard and paste it into a spreadsheet.
• Use a third-party program to extract specific results, such as the program attached to this post: read binary results file (FNO) with a program.
• Edit the Nastran file and manually specify which nodes or elements to print the results. (I have not used this very much, so I am not sure if you can Plot all results so that you see them in the contour and Print selected results to have them in the output file.)