How to make a analysis on oak

Forum|Forum|10 years ago
March 15, 2016
14 replies
3841 views

Dear,

I am trying to make a analysis of a oak beam in Creo ptc.

I draw the beam, made a new material with the oak properties and give it constraint and loads.

But I get strange result out of it if I compare it with other programs like Inventor and Ansys.

I hope somebody can help me.

Thanks beforehands

Kinds regards

Oona

This thread is inactive and closed by the PTC Community Management Team. If you would like to provide a reply and re-open this thread, please notify the moderator and reference the thread. You may also use "Start a topic" button to ask a new question. Please be sure to include what version of the PTC product you are using so another community member knowledgeable about your version may be able to assist.

1_p_beamoakexercise-prt-6.zip

General

Show previous replies

R

rubenvillarreal

14-Alexandrite

Hello,

I am using the Academic Edition so I am able to see the beam.

Check the video for the solution of your problem.

Read while the video is loading...

Solution for Analysis and Simulation Question

Some comments/tips about the video and your problem:

The Academic Version allows to import simulation features from the Lite Version. I use the forces and constraints and create a new analysis. Based on your problem, I though it was better to use a surface and a shell idealization with 48 mm of thickness (in my opinion) and set simulate to 2D Plain Stress.

To avoid point constraints (which can lead to singularities, and personal I don't like it) the two side edges were constrained.

To avoid point forces (which can lead to singularities, and I don't like it either), three edges were sketched and constrained.

Oak is not (by far) an isotropic material, so this is not a valid analysis for this material.

To get the most accurate results, Measures were selected as Convergence Criteria.

Notice how a simple problem reaches the 8th polynomial order when you select Measures as Convergence Criteria. Soon I will post a question about this, when you select Global RMS as convergence criteria, none of the measures (as stress) when you plot it against a graph has a visible convergence, mostly is always a straight line! Why? Notice in the video how convergence was reached by Global RMS and Measures are still to far of 8%. The safety factor will suffer the consequences or your processor should fried?

You are using the Lite Version. Try to apply this tips to your model (eliminate the load on the edges, create little regions or extrudes instead, avoid constraint points..)

Nice Friday to everybody. Sorry for the Spam, was a huge problem upload the video.

U

unickque

1-Visitor

I can't reproduce the 11.4mm now, but that site has some numbers already filled in by default, so that may have caused it.

For a simply supported beam I find 80.8mm. That is also what i find in Creo (81.0mm) and Abaqus (80.9mm) using beam sections on curves.

The difference must be in the constraints on the end points. My beams are "simply supported".

For a beam fully fixed at both ends, the hand calcs say 19.7mm, and Creo says 19.9 mm.

What constraints are you using to obtain 22mm Steven?

U

unickque

1-Visitor

I can't attach files here, so I opened a new Discussion here

There you can find my model, so maybe you can compare to yours?

R

rubenvillarreal

14-Alexandrite

Translating the geometry to the Academic Version and avoiding singularities

Gives the same result. 22 mm. According to the original constraints of the Lite Version, is fixed in all DOF and with free rotation in all direction (SOLID ELEMENTS, which does not support rotation, but well.. just info). Notice the values of Material Properties (KPA!)