Auto-suggest helps you quickly narrow down your search results by suggesting possible matches as you type.

Showing results for

- Navigation
- Simcenter
- Forums
- Blogs
- Knowledge Bases

- Siemens PLM Community
- Simcenter
- 3D Simulation - Femap Forum
- SOLID ELEMENT PRINCIPAL STRESS DIRECTIONS

Options

- Subscribe to RSS Feed
- Mark Topic as New
- Mark Topic as Read
- Float this Topic for Current User
- Bookmark
- Subscribe
- Printer Friendly Page

- Mark as New
- Bookmark
- Subscribe
- Subscribe to RSS Feed
- Highlight
- Email to a Friend
- Report Inappropriate Content

08-25-2016 12:14 PM

I need to be able to determine the principal stress directions to confirm the stress range in a model I am working on, which is subject to tortional and bending load reversal. The model is of a vertical shaft, which is connected to a crank, to which a force is applied such that a CW rotation of 2.16 degrees occurs, followed by a CCW rotation of equal magnitude. Both rotations proceed from a relaxed neutral position. This oscillation occurs at a frequency of 50 hz.

The point of force application on the crank, is 4 inches offset from the center of the vertical shaft so that bending in the shaft is also introduced.

There is a keyway at the top of the shaft and an area at the bottom of the keyway sees a high maximum principal stress when the shaft is rotated CW and the same location sees a cold, if you will, minimum principal stress, when the shaft is rotated in the CCW direction. The opposite side of the vertical keyway sees a similar reversal.

This all makes sense, sense the principal stress planes are at a 45 degree angle to the vertical and forgetting the bending for a moment, the MXP plane for CW would be collinear with the MNP plane for the CCW rotation but I need to show this and include the bending, obviously.

The normal stress, at the surface of the keyway, on which the critical nodes lie should be 0 but is not, (that is another topic), therfore the other two principal stresses should lie in the plane of the keyway surface but that is neither here nor there because I am trying to figure out what the direction cosines mean. Femap yields solid direction cosines labeled as DirCos ij for i & j from 1 to 3, where the first triplet had i as one, the second triplet i as 2, the third i as 3, with j sequenced 1 to 3 for each triplet set.

First of all I am having trouble determining what each triplet represents. I have looked at it a couple of ways. One way was, I took the triplet of DirCos 1j to be unit vectors whose unitized sum was the direction of the maximum principal stress, in effect eigenvector 1 and then the unitized triplet summation of, DirCos 2j, was the direction of the intermediate principal stress, in effect eigenvector 2 and so forth. If this were the case, then I could determine the collinearity or lack thereof of the principal stresses by taking the dot product of the unitized vectors to determine the angle between them. Didn't know whether this was correct or not.

The second way I looked at this was to take DirCos ij, where i and j were equal, to be the direction of Sigma X,Y & Z and DirCos ij, where i and j were not equal, to be the direction cosines of the shear stresses. Didn't know whether this was correct or not either but this interpretation led more or less to the first interpretation.

I know that I could compute the direction cosines algebraically but would prefer not to have to do that and then there is the question of the orientation of the Direction Cosine. Are they to be interpreted as taken with respect to the elemental coordianate system for each element or to be taken with repect to the global coordinate system, which would obviously be more useful. I believe the latter is the case.

One of my pet peeves is that in the Femap and Nastran literature, there is nothing, it least I can find nothing, which defines the principal stress direction cosines with respect to solid elements. The tech guy I spoke to at Siemens support did not have a clue and suggested I Google it.

Can somebody please help?

Regards to all.

brab

Solved! Go to Solution.

3 REPLIES

- Mark as New
- Bookmark
- Subscribe
- Subscribe to RSS Feed
- Highlight
- Email to a Friend
- Report Inappropriate Content

08-25-2016 07:37 PM

Remark 4 of the CHEXA entry from the NX Nastran Quick Ref Guide: "Components of Stress are Output in the Material Coord System".

Remark 4 of the CTETRA entry says the same.

If you use Femap, there's that radio button everyone ignores on the Solid Property dialog, because no one ever changes it (unless,say, wanting cylindrical stress results for pressure vessels). The radio button shows the material coord system is the global coord system.

Thus, direction cosines for solids are with respect to the Basic Rectangular Coord system by default.

If you do vector or tensor plots of principal stresses in Femap, just be careful that these are almost certainly centroidal results, not element corner results - which may explain why you have non-zero surface normal stresses in solids). Other reasons for non-zero normal surface stress results in solids is (a) contact loads; (b) pressure loads; (c) not enough refinement of the modelled detail.

Lastly, to make your job easier, if your primary concern is stresses on the surface of your solid, then consider coating/skinning your solid elements with "very thin" plate elements which effectively act as surface strain gauges, and then all the maths is only 2D instead of 3D.

- Mark as New
- Bookmark
- Subscribe
- Subscribe to RSS Feed
- Highlight
- Email to a Friend
- Report Inappropriate Content

08-26-2016 08:52 AM

EndZ

Thank you for your reply. Yes I do realize that the direction cosines are with respect to the material property's orientation, which in my case is the global coordinate system and that the corner data is unavailable for extraction to the data table, (though it could be made available with a tweak to their software), so I have coverted the corner data to average nodal data so that I could extract it and send it to the data table. I also posited the direction cosines to the nodes. The mesh is refined in the area of the keyway, 1/64th of an inch and yes I have been offered the suggestion of skinning the model, a very laborius procedure. For a sufficiently refined mesh and assuming convergence, the averaging at the nodes should introduce little error.

This type of computation I have to make quite often, utilizing BS 7608 and iiW Hot Spot Stress Analysis as a basis, wherein the specifications require stress range components to be collinear within 45/60 degrees of each other repectively.

I find nowhere in the Nastran documentation where they answer the question I am asking below concerning what each direction cosine represents. There are 9 total direction cosines. Are the first three the components of the eigenvector associated with the Maximum Principal Stress and are the second three the components of the eigenvector associated with the Intermediate Principal Stress and are the 3rd three the components of the eigenvector associated with the Minimum Principal Stress? Maybe the authors of the software take it that this is a nobrainer and that that is obviously what they are?

If the above definition is correct, then the dot product of the eignevectors for the two load cases would define the angle between them.

- Mark as New
- Bookmark
- Subscribe
- Subscribe to RSS Feed
- Highlight
- Email to a Friend
- Report Inappropriate Content

08-26-2016 06:11 PM

Follow Siemens PLM Software

© 2017 Siemens Product Lifecycle Management Software Inc