Autodesk Robot Structural Analysis

[#1]

... | there are no objects that carry the load

This is de warning I'm getting. I think its saying that no elements intersect with the cladding, but the cladding goes through beams, floors and stands on top of a concrete wall.

I tried a correcting with the 'correct' function, but it didnt fix it.

How can I fix this?

(I feel like RSA is sometimes giving me warnings where there shouldnt be one!
Like the warnings 'no material' and 'isolated nodes'. Nodes that have a support are considered isolated??)

[#2]

Try to generate calculation model first and then run verification.

[#3]

---

AlexDT wrote:

... | there are no objects that carry the load

This is de warning I'm getting. I think its saying that no elements intersect with the cladding, but the cladding goes through beams, floors and stands on top of a concrete wall.

I tried a correcting with the 'correct' function, but it didnt fix it.

How can I fix this? (I feel like RSA is sometimes giving me warnings where there shouldnt be one!

Not being able to check your  model I can't tell what is the reason for this warning. If you think it is excessive run model generation and then select the load in which you defined the cladding load. In the attributes dialog mark forces generated automatically and check how they were generated. If they seem to be correct calculate model and check sum of reactions comparing it to the value of load and area of the cladding.

Like the warnings 'no material' and 'isolated nodes'. Nodes that have a support are considered isolated??)

Again make sure that you run model generation before its verification. The supported node is reported as isolated when not attached to any part of the model.

---

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.

[#4]

Thanks both!

Handy function Artur, I can now confirm how the claddingload is distributed! But the warning remains eventhough I see how it is and that it is distributed ?

I dont know how to check the sum of reactions!! 

(I will open a new thread on the isolated nodes)

[#5]

I dont know how to check the sum of reactions!! 

1. Create a separate load case for the cladding load you have issue with

2. Run calculations

3. Open table of reactions and filter it so that only this load case is displayed

4. Check sum of reactions

5. Calculate manually the total value of cladding load you applied

6. Compare values - if the load is correctly applied they should be equal.

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.

[#6]

Thanks, I will do that now.

I started to fixing, but as I trying to fix problems the more problems I get

----------------------------

? Error: Bar length zero

? Error: The element is defined on a story different from the assigned one

? Warning: Faces (the objects without assigned thickness) not used solid area generation. FE mesh has not been generated
? Warning: Distorted element

? Warning: The load has not been distributed correctly | there are no objects that carry the load 

Warning: Incoherent mesh on edges.

Warning: Cohesion of the calculation model has been provided by definition of the kinematic constraints in incoherent points of the finite elements mesh

Warning: The element is defined outside the stories

Warning: the element exceeds geometric limits of the story

Warning: The element is not assigned to any story

---------------------------

[#7]

? Error: Bar length zero

• I've had this before when I'm joining two bars at a position along the bar (ie not at the end point node).  Try to change the model tolerance slightly (more tolerance) and then regenerate the model. 

? Error: The element is defined on a story different from the assigned one

• I would just go to Geometry--------> Stories, and delete all of the levels/stories.  Unless you need story data analysed, it's unnecessary to have the story levels defined.  

? Warning: Distorted element

• Its a problem with the mesh definition I think.  Normally there is some irregularity in the mesh (especially at the joint of two or more panels) that causes this.  It's normally able to be fixed by refining the mesh in that area.  

Warning: Incoherent mesh on edges.

• refine your mesh in that area.  I've experienced this problem due to the tolerance setting (analysis types----------->structure model tab--------------->tolerance of model calculation) being too fine.  Try giving your structure a little more tolerance.  For example, if two panels that join along an edge have slightly different geometry (even by 0.1mm, this can cause the mesh to become incoherent, and it takes a really long time to generate the mesh.  If you change the number of decimals in job preferences, (to say 0.00001) then sometimes you can see slight errors in panel geometry that can cause this issue.  I use Rafals' spreadsheet to fix these errors........http://forums.autodesk.com/t5/Autodesk-Robot-Structural/panel-co-ordinates/m-p/3168358/highlight/tru...

Warning: Cohesion of the calculation model has been provided by definition of the kinematic constraints in incoherent points of the finite elements mesh

• see above

Warning: The element is defined outside the stories

Warning: the element exceeds geometric limits of the story

Warning: The element is not assigned to any story

• delete out all the defined stories as described

tony

---------------------------

[#8]

Thank you Tony for your valuable comments 

Two tips that may help:

1. If your structure is regular try to define structural axes along the walls and at the levels of the floors and use Edit > Detailed Correct with adjusting to structural axes

2. In the meshing parameters go to the detailed options and switch off regular mesh.

These should solve some meshing problems for models with inaccurately defined geometry.

[#9]

Goodmorning! (I live in the Netherlands )

Thanks Tony. I will try your suggestions. I've deleted the stories as you say, so that should be that.

What do you guys recommend for model tolerance as I dont know what this function does exactly? I assume that the model tolerance controls which nodes to merge or something? I'd say 0.2mm instead of 0.1mm.

Ill get back at the other points in a sec.

Thanks Artur.

[#10]

Yes the tolerance just shifts nodes / edges a little to get everything to meet properly.  Just be careful, if you set the tolerance too low (say 10mm), entire beams / panels will visibly shift around.  Then you will have bigger problems than you are currently getting. 

I htink the calculate tolerance button is meant to give you an indication of the ideal tolerance.