Tension members in Staad

Question

Good Day, 
 
 I have attempted the direct analysis method on a steel structure I have to design, however I have the following queries as it relates to the effect tension only members will have on the analysis (the structure has tension rods in the form of X bracing at one side of the building). I have received the following warning and I would like to find out the effect they have on my analysis: 
 1:**WARNING: TENSION/COMPRESSION SPECIFIED WITH PDELTA KG OR 
 DIRECT ANALYSIS. SO TENSION/COMPRESSION IS SWITCHED OFF. 
 2.**WARNING: DIRECT OR PDELTA KG ANALYSIS REQUESTED. 
 SO TENSION/COMPRESSION ANALYSIS IS NOT ALLOWED. 
 
 After I ran my analysis I also realized that my tension members also have compression forces as well, which is quite strange. Any help with these issues would be highly appreciate. 
 
 Thanks.

Sye · Accepted Answer

Gilbert : As of now, STAAD.Pro does not allow Tension/Compression members to be used in a DIRECT ANALYSIS. If TENSION/COMPRESSION is assigned, these attributes are turned off and the members are simply treated as TRUSS members which can take both tension/compression. The warning messages are indicative of that. Also that is the reason why you may get tension or compression in these members. It may be worth noting that the iterative PDELTA analysis, namely PDELTA nn ANALYSIS is the only second order analysis that supports MEMBER TENSION ( or COMPRESSION ) specification.

Sye · Answer

Just for future reference, a wiki is now created on the same topic at 
 communities.bentley.com/.../31875.member-tensioncompression-with-direct-analysis

Sye · Answer

There is no way to run a DIRECT ANALYSIS with MEMBER TENSION. You can do one of the following 
 
Option 1 
Do a DIRECT ANALYSIS with these members specified as TRUSS members. Check the member forces to find out for which load cases the axial forces in these members come out as compressive. Use the INACTIVE MEMBER command to deactivate these members for these cases and rerun the analysis. The members can be active for other cases for which they develop tension force. 
 
Option 2 
Use a PDELTA nn ANALYSIS which supports MEMBER TENSION.

Sye · Answer

I created an example demonstrating how you can use INACTIVE MEMBER specification in conjunction with DIRECT ANALYSIS. Hope this helps. 
 Direct_Analysis_with_Inactive_Members.STD

Sye · Answer

PDELTA ANALYSIS would just do one iteration of pdelta whereas the PDELTA nn ANALYSIS would do "nn" number of iterations of pdelta. The nn stands for the number of iterations. In other words PDELTA 30 ANALYSIS would do 30 iterations. It is always advisable to have a minimum of 15 iterations to check for any possible divergence.

Sye · Answer

Just for future reference. A couple of wikis on the same topic can be found at 
 
 communities.bentley.com/.../31879.direct-analysis-and-member-tension 
 
 communities.bentley.com/.../32145.direct-analysis-with-inactive-members

Sye · Answer

These nodes are actually defined internally by the software as master nodes for the rigid floor diaphragms and hence you did not find these in the model. I noted that the INACTIVE MEMBER specification is triggering the message but I don't think it would have any effect on the analysis as such. I will still check with our development desk on why these are being generated. 
 On a different note, I have a couple of observations regarding your model. 
 You may want to use a SET NL 200 as opposed to SET NL 800 as you have 162 primary load cases only. Setting a very high value is not recommended as it sets aside a lot of additional memory which is not going to be used anyway 
 &hellip; 
 INPUT WIDTH 79 
 *SET NL 800 
 SET NL 200 
 UNIT METER KN 
 Also you may want to take out the member tension commands 
 *MEMBER TENSION 
 *469 TO 474 
 I added the INACTIVE MEMBER 470 471 473 specification instead 
 Also you do not need to do a direct analysis for the seismic cases 1 to 10. PERFORM ANALYSIS after each of the cases 1 to 8 and after the load case 10 should be good. 
 A modified file is attached for your reference. 
 ECFH-Soufriere + Bracing_modified + proper load+ Inactive_modified.std