Modeling CLT

[Anonymous]

Hi all,

I'm looking to model CLT panels. I've done some searching internally (corporate) and externally (forums) and I'm finding little support in this task, so I'm hoping to get some good results from this. At the end of this thread, I'm hoping to be able to model CLT panel in Robot, such that loads can be distributed to multiple edge supports.

I understand from internal documents, where colleagues have modeled CLT in other software packages, that there may be a way to homogonize the materials in the two principle directions of the plane of the panel, and then to come up with coefficients (n1 and n2 in Panel>Thickness ... > Othotropic >material orthotropy). I'm not sure if this is this method of modeling the panel thickness will allow for analysis of all the strength and serviceability criteria.

Another possible solution is to do a user-defined material, and to manually define the stiffness matrix. This is a rather complex route, but I'm open to trying to figure it out.

If anyone has experience with either of these methods, or is also interested in figuring it out, let's chat!

Cheers

[Anonymous]

To keep this moving forward, I think that the most appropriate method is to define a material using the material orthotropy settings (manually define a matrix). The Autodesk Robot documentation on this is quite poor --- it could use a good revision. There are also some special considerations with CLT elements, so I'm hoping to get some additional input, if anyone has any.

Cheers

[Artur.Kosakowski · Accepted solution]

You may find this helpful:

https://forums.autodesk.com/autodesk/attachments/autodesk/2053/1646/1/15.02.20_StiffenssMatrix.pdf

If you find your post answered press the Accept as Solution button please. This will help other users to find solutions much faster. Thank you.

[Artur.Kosakowski · Accepted solution]

http://forums.autodesk.com/t5/robot-structural-analysis/construction-en-panneau-bois-clt/td-p/567380...

If you find your post answered press the Accept as Solution button please. This will help other users to find solutions much faster. Thank you.

[Anonymous]

You're a saint! Thanks for this. The PDF looks extremely promising (I'm going to delve into it now), and the French article is exactly what I was looking for in English. I was kind of surprised no one had asked the question already, but now I see that it's just that no one asked in English.

I will follow up with marking as a solution or further questions if necessary, shortly.

Cheers

[Anonymous]

So these resources have been great. I have just one question about the Robot inputs shown in that French thread:

What are the thickness inputs? In the screenshots shown the numbers input to the Th, Th 1, Th 2 input boxes are completely arbitrary as far as I can tell (they're showing the inputs for a 182mm panel, but they have 16 cm and 25 cm input...

Can we shine a light on that?

Mike

[Artur.Kosakowski]

http://help.autodesk.com/view/RSAPRO/2017/ENU/?guid=GUID-2000B438-5453-4C90-B658-E3DE6F8AF33A

If you find your post answered press the Accept as Solution button please. This will help other users to find solutions much faster. Thank you.

[Anonymous]

Okay, that's fair. I suppose the input values in that screenshot are in fact arbitrary or unrelated to the example.

So Th is necessary for self-weight: I guess this is necessary for the shell bending and shear calcs, and I'm forced to let Robot calc the panel self-wt?

And Th 1 and Th 2 are unnecessary unless I'm dealing with thermal gradients?

Cheers

[Artur.Kosakowski]

So Th is necessary for self-weight: I guess this is necessary for the shell bending and shear calcs, and I'm forced to let Robot calc the panel self-wt?

Yes, this will be the value used for automatic self-weight calculations when you include this panel in the list for such type of load.

And Th 1 and Th 2 are unnecessary unless I'm dealing with thermal gradients?

Correct.

If you find your post answered press the Accept as Solution button please. This will help other users to find solutions much faster. Thank you.

[Anonymous]

Thanks again for your help Artur. I have been able to figure out a stiffness matrix, define a user-defined orthotropic material, and to define an orthotropic direction.

I have been modeling a simple 5m CLT span with 2.0kN.m DL and 2.0kN.m LL, to verify that the results are coming out as expected. I have had reasonable success: if I play around with the Map settings enough, I find the expected maximum shear and moment forces (14.25kN and 17.81kN.m) (Note: by "play around" I mean I have to select orientations that aren't always what I would expect). Also, the expected maximum shear stress is right. However, the expected maximum bending moment is about 70-80% of the expected value, according to the Maps; and by Tables, whereas the shear and moment forces and shear stress are coming out as expected, the bending stress is only ever showing 0.0... I've tried  playing with different directioning as well -- no luck.

Furthermore, the deflection is off by several orders of magnitude.

I think some of this has to do with a problem with the panel vs FE local axes. I found a similar problem in a much earlier forum posting, from several years ago. I have in fact selected the entire panel, and manually defined the Local System Orientation (Geometry > Properties > Local system Orientation > {Direction vector of X-axis: 1,0, 0} > Apply) but on closing that window, the FE local axes reorient, displaying X- in the [0 -1 0] direction.

In summary: there are several ongoing Results problems that I suspect are related to the definition of the local FE axis definition, but perhaps there is more... I've attached the Robot file for your review.

[Artur.Kosakowski]

However, the expected maximum bending moment is about 70-80% of the expected value, according to the Maps; and by Tables,

 the bending stress is only ever showing 0.0...

If you find your post answered press the Accept as Solution button please. This will help other users to find solutions much faster. Thank you.

[Anonymous]

Okay, that covers one of the output problems (Thanks). I am getting used to the fragmentation of the maps results and the table results. I expected the table results to be more closely aligned with the settings of the maps, so I hadn't thought to adjust the parameters you've shown here.

Anyways, that local axis orientation is an ongoing challenge. If that's fixed, I wonder if the bending stress (10.69MPa) will increase to the predicted (13.49MPa). However, I suspect this also has more to do with the section properties used in a manual CLT bending stress calc (I=Ieff, excludes transverse layers) whereas Robot is using a different moment of inertia in the panel section.

[Anonymous]

Okay, that covers one of the output problems (Thanks). I am getting used to the fragmentation of the maps results and the table results. I expected the table results to be more closely aligned with the settings of the maps, so I hadn't thought to adjust the parameters you've shown here.

Edit: 10.69MPa is the result you would get if you considered the gross cross-section, instead of just the effective cross-section. I think I'll need to come up with a clever solution to get it to do the effective moment of inertia. I'm still learning and trying to work this out on my own.

Edit: Anyways, that local axis orientation is an ongoing challenge. If that's fixed, I wonder if the deflection results will be fixed (currently showing 1604mm max deflection under the SLS cases). I suspect this won't solve the deflection problem... But it needs to be fixed still.

[Artur.Kosakowski]

Edit: 10.69MPa is the result you would get if you considered the gross cross-section, instead of just the effective cross-section. I think I'll need to come up with a clever solution to get it to do the effective moment of inertia. I'm still learning and trying to work this out on my own.

What about modifying the thickness th value? 

Edit: Anyways, that local axis orientation is an ongoing challenge. If that's fixed, I wonder if the deflection results will be fixed (currently showing 1604mm max deflection under the SLS cases). I suspect this won't solve the deflection problem... But it needs to be fixed still.

Anyways, that local axis orientation is an ongoing challenge. If that's fixed,

I'm not sure what you mean.

---

[Anonymous]

Modifying the th value would also affect the self-weight, so --- it's a possibility that I come up with a coefficient between I_gross and I_eff (where the former is the total cross section and the latter is just the longitudinal CLT layers) but then I have to accommodate for the self-weight problem. If there is an override for the moment of inertia value, that would work (I'm coming from a SAP2000 background, and that's how I would address it in that package).

Regarding the local axis directions, the screenshots below should help. Note: I have payed with some of the panel local coordinate settings (as per the original post).

Local system of panels shows x-axis in global x-axis direction (this is what I want)

FE Local System shows x-axis going in the global negative-y direction

[Artur.Kosakowski]

Modifying the th value would also affect the self-weight, so --- it's a possibility that I come up with a coefficient between I_gross and I_eff (where the former is the total cross section and the latter is just the longitudinal CLT layers) but then I have to accommodate for the self-weight problem. If there is an override for the moment of inertia value, that would work (I'm coming from a SAP2000 background, and that's how I would address it in that package).

As you know the unit weight of the panel just exclude it from the automatically generated self-weigh and replace it with the corresponding uniform surface load. 

Regarding the local axis directions, the screenshots below should help. Note: I have payed with some of the panel local coordinate settings (as per the original post).

Local system of panels shows x-axis in global x-axis direction (this is what I want) 

And this is the display you should look at.

FE Local System shows x-axis going in the global negative-y direction

It is just informative and is based on the order of creation of the surface element nodes. It is not used for neither any attribute assignment nor loads or results display. In other words there is no reason to display it as it will not be 'used' anywhere.

If you find your post answered press the Accept as Solution button please. This will help other users to find solutions much faster. Thank you.

---

[Anonymous]

Okay. On one hand, this is good news -- but that means I'm running out of ideas for the deflection problem.

Since the deflection is a function of load, length, stiffness, and moment of inertia --- and so far I've confirmed from all these other results that load, length, and moment of inertia are what I expect --- it leaves stiffness as a possible source of the huge deflection overestimate (1604mm under the SLS- case, where I expect it to be: 5/384 * 4.0 * 5000^4 / E I = 31mm). I manually calculated the orthogonal stiffness matrices using the Stora Enso document provided by your earliest posts, and they are consistent with the tabulated stiffness matrices in the document itself. So... I'm going to have to scratch my head for a bit and think about this.

[Artur.Kosakowski]

I'd double check the values of the stiffness matrix. It may make sense to compare with the standard timber panel to see the range of the values to exclude 'big' mistakes (like units) first.

 

If you find your post answered press the Accept as Solution button please. This will help other users to find solutions much faster. Thank you.

[Anonymous]

I'm investigating this now. I considered units earlier, but the Stora Enso doc (and my inputs) are consistent with the Robot default input units (kN.m) as per the Stiffness Matrices dialogue.

Comparing the 'standard' timber panel and this CLT panel: It's not a consistent order of magnitude difference between the input values (i.e. some are off by a factor of 10, and others by 100,000). For the sake of trying, I increased the magnitudes (D matrix * 1000, K*10, H*100,000). This resulted in a more "reasonable" deflection of ~4mm, but still a far cry from the 31mm expected.

[Anonymous]

Solved. Orders of magnitude changed in various ways... I have no idea why, and I'll have to explore that a bit, but the StoraEnso matrix output orders of magnitude won't work in the Robot input panel.