# Timber modeling (engineering constants) **URL:** \ **Category:** General Questions\ **Created:** [September 26, 2023, 5:46pm UTC](https://prepomax.discourse.group/t/timber-modeling-engineering-constants/1120 "2023-09-26T17:46:53Z")\ **Posts on this page:** 12\ **Page:** 1
**Author:** ![E.Martin](https://avatars.discourse-cdn.com/v4/letter/e/e47c2d/32.png) [@E.Martin](https://prepomax.discourse.group/u/E.Martin)\ **Post date:** [September 26, 2023, 5:46pm UTC](https://prepomax.discourse.group/t/timber-modeling-engineering-constants/1120/1 "2023-09-26T17:46:53Z")
I have considered modeling a simple cylindrical piece of wood in tension. I think that the definition of the material should be using ENGINEERING CONSTANTS, indicating different coefficients according to the longitudinal and radial directions, according to: first line: E1,E2,E3,v12,v13,v23,G12,G13, second line: G23,T I understand that it could be like this: \*Material, Name=oak \*Elastic,Type=ENGINEERING CONSTANTS 11300000000.0,1740000000.0,1740000000.0,0.369,0.369,0.618,1005000000.0,1005000000.0 915000000.0,20.0 \*Density 700.0 \*Solid section, Elset=timber, Material=oak These lines have been entered with the “Edit CalculiX Keywords” option. Could someone tell me how I can ensure that the 1,2,3 directions with which the constants are defined correspond in the finite elements to the global Z,X,Y directions of the model? Thank you very much in advance for your attention. ![SNAG-0000](https://global.discourse-cdn.com/free1/uploads/prepomax/original/2X/b/bdffc3d3efb80d24931e58fef6817a213c7be5e6.png) ---
**Author:** ![FEAnalyst](https://yyz2.discourse-cdn.com/free1/user_avatar/prepomax.discourse.group/feanalyst/32/688_2.png) [@FEAnalyst](https://prepomax.discourse.group/u/FEAnalyst)\ **Post date:** [September 26, 2023, 5:58pm UTC](https://prepomax.discourse.group/t/timber-modeling-engineering-constants/1120/2 "2023-09-26T17:58:52Z")
By default, this is the case but you could use the \*ORIENTATION keyword to change it. How to check it ? Just load the model (possibly a cube) in different directions and check the displacements. ---
**Author:** ![E.Martin](https://avatars.discourse-cdn.com/v4/letter/e/e47c2d/32.png) [@E.Martin](https://prepomax.discourse.group/u/E.Martin)\ **Post date:** [September 26, 2023, 6:11pm UTC](https://prepomax.discourse.group/t/timber-modeling-engineering-constants/1120/3 "2023-09-26T18:11:39Z")
Should I understand that the local axes 1,2,3 refer to the part, not to each finite element separately? ---
**Author:** ![FEAnalyst](https://yyz2.discourse-cdn.com/free1/user_avatar/prepomax.discourse.group/feanalyst/32/688_2.png) [@FEAnalyst](https://prepomax.discourse.group/u/FEAnalyst)\ **Post date:** [September 26, 2023, 6:17pm UTC](https://prepomax.discourse.group/t/timber-modeling-engineering-constants/1120/4 "2023-09-26T18:17:09Z")
Each element uses global (or local if specified) directions. You could run a single element test (with one hex element) to see how it works. That’s the best way to check and understand material behavior. ---
**Author:** ![FEAnalyst](https://yyz2.discourse-cdn.com/free1/user_avatar/prepomax.discourse.group/feanalyst/32/688_2.png) [@FEAnalyst](https://prepomax.discourse.group/u/FEAnalyst)\ **Post date:** [September 26, 2023, 6:30pm UTC](https://prepomax.discourse.group/t/timber-modeling-engineering-constants/1120/5 "2023-09-26T18:30:21Z")
Visualization from Abaqus (of course, 1=X, 2=Y, 3=Z): ![vis](https://global.discourse-cdn.com/free1/uploads/prepomax/original/2X/d/d00aef2ab33a164fe6d5a7dc6d78e63375853ab9.png) ---
**Author:** ![E.Martin](https://avatars.discourse-cdn.com/v4/letter/e/e47c2d/32.png) [@E.Martin](https://prepomax.discourse.group/u/E.Martin)\ **Post date:** [September 26, 2023, 6:32pm UTC](https://prepomax.discourse.group/t/timber-modeling-engineering-constants/1120/6 "2023-09-26T18:32:22Z")
Is there a way to visualize those local element orientations in PrePoMax? Thank you very much for your help. My problem is that, if I have to assign a local system to the elements with ORIENTATION, I should know what the proper axes of each one are like, right? ---
**Author:** ![FEAnalyst](https://yyz2.discourse-cdn.com/free1/user_avatar/prepomax.discourse.group/feanalyst/32/688_2.png) [@FEAnalyst](https://prepomax.discourse.group/u/FEAnalyst)\ **Post date:** [September 26, 2023, 6:37pm UTC](https://prepomax.discourse.group/t/timber-modeling-engineering-constants/1120/7 "2023-09-26T18:37:59Z")
No, because ortho- and anisotropic materials and thus also local orientations are not yet supported in PrePoMax. Check how \*ORIENTATION is defined. You just specify the coordinates of 2 points forming a new coordinate system to be used for the whole element set (e.g. for the whole part). Normally, it’s not necessary to add spatial variation to this. ---
**Author:** ![E.Martin](https://avatars.discourse-cdn.com/v4/letter/e/e47c2d/32.png) [@E.Martin](https://prepomax.discourse.group/u/E.Martin)\ **Post date:** [September 26, 2023, 6:51pm UTC](https://prepomax.discourse.group/t/timber-modeling-engineering-constants/1120/8 "2023-09-26T18:51:01Z")
I have created 3 cubes, with the same material and loading and support conditions, but using ORIENTATION so that the greatest rigidity varies from one to another. And what I get is absolutely zero results. The problem comes from ORIENTATION, since if it is not included it does offer results (obviously the same in all 3 cases). Do you have any ideas about what I’m doing wrong? \*Material, Name=test \*Elastic,Type=ENGINEERING CONSTANTS 1000.0,500.0,500.0,0.2,0.2,0.3,500.0,500.0 250.0,20.0 \*Orientation, Name=orientationZ, System=RECTANGULAR 0.,0.,1.,1.0,0.,0. \*Orientation, Name=orientationX, System=RECTANGULAR 1.,0.,0.,1.,0.,0. \*Orientation, Name=orientationY, System=RECTANGULAR 0.,1.,0.,0.,0.,1. \*Solid section, Elset=Solid\_part-1, Material=test, Orientation=orientationZ \*Solid section, Elset=Solid\_part-2, Material=test, Orientation=orientationX \*Solid section, Elset=Solid\_part-3, Material=test, Orientation=orientationY ![SNAG-0000](https://global.discourse-cdn.com/free1/uploads/prepomax/original/2X/c/c59f576d05a56efa022fa9521e73c46720f83fcf.png) [cubes.inp](https://prepomax.discourse.group/uploads/short-url/rfOqx3988KBergF47AQiX5f9ipc.inp) (4.1 MB) ---
**Author:** ![FEAnalyst](https://yyz2.discourse-cdn.com/free1/user_avatar/prepomax.discourse.group/feanalyst/32/688_2.png) [@FEAnalyst](https://prepomax.discourse.group/u/FEAnalyst)\ **Post date:** [September 26, 2023, 7:10pm UTC](https://prepomax.discourse.group/t/timber-modeling-engineering-constants/1120/9 "2023-09-26T19:10:55Z")
> [@E.Martin](#): > > \*Orientation, Name=orientationX, System=RECTANGULAR > 1.,0.,0.,1.,0.,0. This one is incorrect because it uses the same coordinates for both points. ---
**Author:** ![E.Martin](https://avatars.discourse-cdn.com/v4/letter/e/e47c2d/32.png) [@E.Martin](https://prepomax.discourse.group/u/E.Martin)\ **Post date:** [September 26, 2023, 7:15pm UTC](https://prepomax.discourse.group/t/timber-modeling-engineering-constants/1120/11 "2023-09-26T19:15:10Z")
You are absolutely right, I didn’t see it! Thank you so much! ---
**Author:** ![tsvilans](https://yyz2.discourse-cdn.com/free1/user_avatar/prepomax.discourse.group/tsvilans/32/516_2.png) [@tsvilans](https://prepomax.discourse.group/u/tsvilans)\ **Post date:** [October 1, 2023, 1:28pm UTC](https://prepomax.discourse.group/t/timber-modeling-engineering-constants/1120/12 "2023-10-01T13:28:06Z")
You can further define per-element orientation using the `*DISTRIBUTION` card, followed by element ID and the 2 axes (X- and Y-axes). I have used this to model the changing material orientation through - for example - a log with knots. ---
**Author:** ![E.Martin](https://avatars.discourse-cdn.com/v4/letter/e/e47c2d/32.png) [@E.Martin](https://prepomax.discourse.group/u/E.Martin)\ **Post date:** [October 2, 2023, 8:02am UTC](https://prepomax.discourse.group/t/timber-modeling-engineering-constants/1120/13 "2023-10-02T08:02:01Z")
Thank you very much for your contribution. I will try it