Instability type 3

[Anonymous]

I have Type 3 Instability in my model and I read this thread: http://forums.autodesk.com/t5/Autodesk-Robot-Structural/instability-type-3-RX-direction/m-p/3364875

Now, I do not think I have any extremely short members, because "Tolerance of  structure model generation" is set to 30 mm. There are no rigid links, diaphragms, etc. Also the results are correct, so I don't think there is any mechanical instability. The longest member is 12 meter long. Is it possible that stiffness difference between a 30mm member and 12,000mm member triggers Type 3 Instability message or it must be something else?

[Rafal.Gaweda]

Send us this model to check

[Artur.Kosakowski]

Yes, this is possible especially when a 30mm bar has got a large section and the 12 m a small section assigned. You may try to make a quick test and assign the same section to all bars. If it is only the size of the sections that causes the very large difference in the stiffness then the instability will no longer be reported. Please mind that this may not be enough (to get rid of the  instability warning) in cases the difference in lengths is too large.

[Anonymous]

Sorry fot the late response, I was on vacation.

As Artur suggested, I did a small test and applied the same section to all members and then the Istability type 3 warning did not show up.

I am trying to figure a way to solve this problem: Would it help to divide long members into shorter members?

Rafal, I have sent you the model.

[Artur.Kosakowski]

No, this will probably not help. Form what you wrote I'd say that you can just ignore the warning (unless you want to use similar sections for all bars of the model) after carefully checking the deformation shape of the structure under applied load as well as values of nodal displacements and rotations.

[Rafal.Gaweda]

I am trying to figure a way to solve this problem: Would it help to divide long members into shorter members?

Rafal, I have sent you the model.

---

I guess if you enhance geometry accuracy in your model it willbe fine.

Check this: on dummy model select everything and make intersection, open Bars table on Values tab, sort it by length,

find the shortest ones, correct these places on original model.

[Anonymous]

Should not "Tolerance of structure model generation", which is set in this case to 30mm, take care of this and assure that no element is shorter than 30mm?

[Rafal.Gaweda]

I would suggest to correct geometry manually \ by Correct options in Robot or to correct analytical model in RST.

[Anonymous]

Patrick,

I would be careful using 30mm as model tolerance, as every time you recalculate the structure nodes/panel edges will move and therefore you will need increasingly larger tolerance every time.  

Tony

[Anonymous]

Rafal,

Now I am not sure if I understand what "Tolerance of structure model generation" does. Is it not supposed to merge any nodes that are less than 30mm apart?

[Anonymous]

Tony,

Why do you think that nodes/edges will move after each calculation? Maybe I am missing something, but I would think that all inaccuracies are corrected during the first run and during later calculations there is nothing to correct, so nodes will not move. Could you please elaborate on this behavior?

[Anonymous]

Hi Patrick

Indeed you are correct in that once the model is "corrected" it will remain in this position and therefore not require further moving.  The problem I have encountered is this (sample case):

1. Set up a model with many panels (say 100).  Vertical and horizontal panels, all kinds of geometry (not necessarily rectangles);
2. Some geometry may be out by a few points of a mm;
3. Robot automatically "corrects" these small discrepancies;
4. I then try to mesh panels.  Maybe a wall here or there does not mesh, due to some panels being "warped" etc;
5. I then delete out offending non-meshing panel and re-draw it.  Since the adjoining panel was shifted due to "model correction" (step 3), it now is not matching my newly drawn one (step 5).  
6. The panel already shifted in step 3 now shifts again to match the new panel in step 5.  You can see that at an intersection of 4 or 5 panels this becomes very tiresome when one or two panels will just not mesh no matter what.  Each time I delete and re-draw a panel, 4 other panels shift to accomodate it.  So I say "OK, I'll just run more tolerance", and set tolerance to 10mm.  
7. I now have many panels "warped" to suit the adjoining one by up to 10mm but still no better off trying ot mesh everything beautifully, and I also have many panels visilbly out of alignment.  
8. Meshing the intersections of all of these slightly "out" panels takes forever is is not useful for calculation anyway.  

Hope this helps explain better to you the issues I've come across.

 My workflow is now thus;

1. As soon as I open a new model I set tolerance to ZERO;
2. Build model (either from Revit import or build in Robot);
3. Run Rafal's magic spreadsheet (search forum) and make sure my geometry is EXACTLY how I want it;
4. Then mesh and run the model generation.

 This is why I have been pushing Autodesk development (via this forum) to allow Robot to round element dimensions to the same number of decimal points as the overall units setting.  It will avoid having numbers such as 2.000054876 that just show up as 2.000 in the object inspector etc (which is the starting point for 99% of all meshing problems / slow calculation time / general frustration I experienced in Robot).  

For the benefit of others who have not experience this I have attached a PDF explaining the situation graphically.  

Tony

[Artur.Kosakowski]

Tony,

Rounding coordinates seems to be smart solution but unfortunately it is not (good for planes that are parallel to the main coordinate system but fails badly for sloping ones - we have tried this approach ). What I would recommend is:

1. Freeze the meshes of the panels that you are pleased with before correcting the geometry of the model (meshes of not frozen or not meshed panels will try to adopt to the position of nodes of the existing meshes).

2. Use adjust to plane / structural axes correction rather than increase the model tolerance. This is the powerful tool yet intended to be used in specific cases (when you know what a change is going to be and it is a local adjustment of the model) rather than to be applied blindly to a complex model where you are not able to check what unwanted effect it can possibly have.

BTW: After running bar intersections to determine the shortests bars check if they exist due to the inaccuracy in the model or just because of the intended positions of other bars or objects in the model. Very often this (3 cm bar) is just the feature of the model itself rather than the lack of accuracy. Please mind the check Patrick made:

As Artur suggested, I did a small test and applied the same section to all members and then the Istability type 3 warning did not show up.

[Rafal.Gaweda]

1. Run Rafal's magic spreadsheet (search forum) and make sure my geometry is EXACTLY how I want it;

Not only mine Tony. Do not be so modest !

http://forums.autodesk.com/t5/Autodesk-Robot-Structural/Panel-contour-points-modification-API/td-p/3...

Check also:

http://forums.autodesk.com/t5/Autodesk-Robot-Structural/Rounding-up-coordinates-API/m-p/3430533/high...

http://forums.autodesk.com/t5/Autodesk-Robot-Structural/API-addin-checking-flatness-of-panels-contou...

[Anonymous]

I read with great interest your posts guys and now I understand what problem Tony was referring to.

But, my question as related to short members and type 3 instability was left unanswered...

---

Now I am not sure if I understand what "Tolerance of structure model generation" does. Is it not supposed to merge any nodes that are less than 30mm apart?

---

How is it possible that after model generation I would still have elements shorter than 30mm?

[Artur.Kosakowski · Accepted solution]

Now I am not sure if I understand what "Tolerance of structure model generation" does. Is it not supposed to merge any nodes that are less than 30mm apart?

---

True, but not e.g. calculation nodes. Please try to follow these steps:

1. Select all model (CTRL+A) and run intersection (Edit > Intersect)

2. Find the shorter bars and determine why their end nodes are in such locations

Knowing this I believe you should be able to answer your question

[Anonymous]

Ok, I see what happens. The end nodes get snapped together. But if there are elements coming into other elements in between nodes, they are not adujsted, only calculation nodes are created at the intersections.

[Anonymous]

Hi,
 
I have been trying to fix the warnings (Separate Structure and instability type 3) for couple of days. However, I could not find a way to fix it by following the procedures in both forums (Separate Structure and instability type 3) because the instability type 3 is changing from node to node!!! (Starting from Node 2053, 2012, to finally 1961 for the last run). So, Please help me if you can as the file is attached.
 
Appreciate any help.

[muhammadhilmi1006]

I have an problem instability (type 3) in my model, can you help me to find a solution to the problem? thank you