Tension Only member with one UBC case

If MEMBER TENSION is specified, it is considered for all cases. Not sure why you mentioned that it is only considered for the first seismic case. For example, if you look at the second seismic case ( load case 2 ) in your model, the bracing 110 shows a tension force while the member 109 shows zero force. The member 109 shows zero force because the member has been switched off from the analysis as it would develop compression under the load 2. So the MEMBER TENSION command is active for load case 2 and for all subsequent cases.

The PERFORM ANALYSIS and CHANGE commands that you have used after load case 17 to 32 are redundant and it is fine to use one PERFORM ANALYSIS and CHANGE after load case 33.

You used a ACC 0.05 but unless you include the accidental torsion as part of the seismic definition, the accidental torsion would not be included. Also use ACC as 1 in this case as the software would internally consider 5% of the building dimension as the accidental eccentricity. What you are specifying here is a multiplication factor for that calculated accidental torsion. So you need to specify

DEFINE IBC 2012 ACCIDENTAL

SS 0.75 S1 0.3 I 1 RX 3 RZ 3 SCLASS 2 TL 12 FA 1 FV 1

…

…

LOAD 1 LOADTYPE Seismic  TITLE SX

IBC LOAD X 1 ACC 1

…

Also depending on which load cases you would like to design against, you may want to use a LOAD LIST command ahead of the PARAMETER 1 to restrict the design to such cases.

Thank you, but I have some questions:

1- Why I can't add any repeat load after load case 33 and it shows some error.

2- When I have to use CHANGE & PERFORM ANALYSIS multiple time ?

3- Tension force at the tension-only member appears in wired shape ( triangle shape at the ends and zero along the member ) did you face such case.

1. For models involving multiple analysis commands, if the number of primary load cases exceed 40, one needs to add a SET NL nn command before the Joint Coordinates, letting the software know how many primary cases are going to be solved during the analysis. The nn stands for the total number of primary load cases ( includes REPEAT LOADs). This allows the software to set aside the appropriate amount of memory for the analysis. Here is a sample

STAAD SPACE
START JOB INFORMATION
ENGINEER DATE 16-Nov-16
END JOB INFORMATION
INPUT WIDTH 79
SET NL 100
UNIT METER KN
JOINT COORDINATES
...

2. PERFORM ANALYSIS and CHANGE has to be used after each generated seismic case in your model as these have been later used in REPEAT LOADs. Unless your MEMBER TENSION specifications are changing ( like you are not using different sets of members as tension only for different cases ) using the PERFORM ANALYSIS and CHANGE once at the very end is fine. On the other hand if the MEMBER TENSION specifications are different for the load cases, each load would have to be followed up by a PERFORM ANALYSIS and CHANGE followed by the new MEMBER TENSION specification.

3. There was a glitch in earlier versions of the program which caused the axial force diagram to be plotted incorrectly, as you noted, for truss/tension members. It has seen been addressed since then. I think it was fixed in STAAD.Pro 20.07.11.50. So I would suggest that you use the latest STAAD.Pro 20.07.11.82 and you should not face this issue.