ETABS 9.7.4 Runtime Error Message

[EngrUzair]

AA. I am analysing a  2B+10 RC structure, located in seismic zone 2B on ETABS 9.7.4.

The image showing the runtime error, displayed by the software is attached below this post.

My questions are as under:

a. Why might be the source or reason of this error?

b. More importantly, how the affected element (indicated by the number 22836 in the attached image) can be located in the ETABS model?

An urgent help is needed to sort out above problem.

Regards.

Edited September 17, 2017 by EngrUzair

[tachauhan]

Salam, just remesh the stucture with different max element size so that problematic element get relocated. Hope this quick fix would solve the problem. Otherwise post the model for probing in.

Regards

tachauhan

[UmarMakhzumi]

Dear Uzair Sb,

The error is in slab element 22836. You can find that element by looking at respective story level. For that, you will need to turn on the Area Labels and use the X, Y and Z Coordinates provided in the error log. Solution to the problem is to either re-mesh the area manually for that part or to do the load distribution manually and directly apply load at beams and just delete the slab.

Please let us know if the problem has been fixed or otherwise.

Thanks.

[EngrJunaid]

Dear Sir,

The option of selection any element by its UNIQUE NAME is available in ETABS v13 but unfortunately we don't have this selection option in ETABS v9.

Display the meshing from set building view option and check the irrigular meshed area by right clicking on them for the effected area.

All the WARNINGS are shown in the last Analysis Log with the global co-ordinates of the effected element.

From those co-ordinates the area creating problem can be easily found.

 

Thanks 

[WR1]

The first step towards obtaining the stiffness matrix, is to obtain the Jacobian, using an equation which you can find in any finite element analysis book. This equation has a shape function matrix which depends on the nodal displacements. 

Once Jacobian obtained, the strain displacement matrix is obtained and transposed and then finally stiffness matrix is obtained.

Jacobian will be negative if there are distorted elements, local axis of connected elements is different etc. Check element 22836. If you cannot find this in ETABS 9.7, then do this to find coordinates.

Display > Show Tables > Model Definitions > Area Assignments > Area Assignment Summary

Then export to EXCEL, find area 22836, and then within the same row, look for centroidx and centroidy coordinates.

[EngrJunaid]

Sir the simplest & easiest way of finding the area by its unique name is ETABS v13.

Open your model in ETABS v13, go to Select ---->  Labels ----->  Shell Unique Name ----> enter the name of the required area.

[WR1]

20 hours ago, EngrJunaid said:

Sir the simplest & easiest way of finding the area by its unique name is ETABS v13.

Open your model in ETABS v13, go to Select ---->  Labels ----->  Shell Unique Name ----> enter the name of the required area.

Yes, but my post was, how to do this in ETABS 9.7 if some one doesnt have v13.

[Saad Pervez]

On 9/17/2017 at 6:58 PM, UmarMakhzumi said:

Dear Uzair Sb,

The error is in slab element 22836. You can find that element by looking at respective story level. For that, you will need to turn on the Area Labels and use the X, Y and Z Coordinates provided in the error log. Solution to the problem is to either re-mesh the area manually for that part or to do the load distribution manually and directly apply load at beams and just delete the slab.

Please let us know if the problem has been fixed or otherwise.

Thanks.

Slab element number during analysis and slab area labels are different. Slab number during analysis is the position of that element in the database, slab area labels have the notation F### and usually indicate when this particular element was drawn, slab area labels can also be repeated in different stories, slab element number is unique.

On 9/19/2017 at 9:24 AM, Rana said:

Then export to EXCEL, find area 22836, and then within the same row, look for centroidx and centroidy coordinates.

Exporting to EXCEL will also not help because EXCEL will slab area labels, not slab element number.

Exporting the model to .e2k and the importing it back might help, OR you can do a manual check of all your model by studying the mesh. In my experience, this error is caused by a shell element with 2 nodes only, which happens when you move one set of points to already existing points by move command, this will merge the points but the element defined between them stays in the database.

Hope this helps.

 

[EngrUzair]

AA. Here is the progress & update regarding the problem described in my original post, for the benefit of the interested SEFP users.

1. Automeshing was adopted in the original ETABS 9 model, with a maximum mesh size of 3 ft for the slabs & walls. The slabs included a raft slab as well, for tranferring the reactions to SAFE.

2. The model was being updated in steps, by refining the geometry along various edges of the slabs according to architectural plans at different floors. Model was running fine at all the steps.

3. The problem most probably occurred when the whole model (including the raft slab) was selected through 'Select all' command & automeshed again as stated in para-1 above. This action meshed the raft slab as well.The meshing of raft slab was haphazard in some regions, because of orientation of slab outer edges in different directions.

4. Following steps were taken in order to sort out the error:-

a. Trials were made by automeshing the model at two different maximum mesh sizes of 4 ft & 2 ft (one at a time), but without any positive result.

b. Third trial was made using 'default' meshing option ( meshing at grids & in Automesh options, by keeping the 'Further subdivide shell/wall in maximum element size of' option UNCHECKED. This trial helped in running the analysis completely, with 2 Warning Messages indicating presence of unconnected point & frame objects at the specified locations. Deletion of these extra objects removed the warning messages.

c. Another trial indicated that thr problem is with the meshing of slabs, and not the walls.  

d. Trying to locate affected element # 22836 through the procedure advised by Rana, indicated that the relevant output table designates the slab & wall elements by the number types F### for slab elements & W### for wall elements. It followed that element numbers (like 22836 etc) are generated during analysis only. The same facts have been stated above by Saad Pervez. Thus, the affected element could not be traced once again.

e. Keeping in view suggestion made by EngrJunaid, the affected model was opened in ETABS 2016. This time the affected element was located & found to be present in the automeshed Raft Slab, provided at the base level merely for exporting the Base Reactions to SAFE for further processing there. 

5. Replacing the affected Automeshed Raft Slab, with a new unmeshed raft slab & remeshing the floor slabs & rc walls (after selecting the floor slabs & walls separately) at desired maximum mesh size finally solved the problem.

In the end, thanks to all (especially @EngrJunaid) for contribution to reach the solution of subject problem, by suggesting various courses of action.

Regards.

 

Edited September 25, 2017 by EngrUzair

[Salman Shamim]

most of the time this error is caused by irregular behavior of shells having nodes near to each other. A quick fix which works most of the time for me is i select whole model and from edit menu- merge point, increase merge point tolerance (say 6").