chia sẻ về PHÂN TÍCH INPLACE trong phần mềm sacs

Thảo luận trong 'SACS SOFTWARE' bắt đầu bởi manhcuongcb2, 16/11/16.

  1. manhcuongcb2

    manhcuongcb2 New Member

    Tham gia ngày:
    Bài viết:
    Đã được thích:
    Điểm thành tích:
    Giới tính:
    mình mạn phép chia sẻ một ít tài liệu cho bạn nào cần về phần mềm SACS.
    Chủ đề chia sẻ về hướng dẫn sử dụng sacs trong phân tích thiết kế JACKET.
    phân tích inplace đòi hỏi kết hợp mô hình jacket và topside phải được tạo ra trong sacs:
    các bước như sau:
    1. Define the basic Jacket framing using the Jacket wizard in Preceed-Pro which defines the leg batter, conductor spacing and leg and/or skirt pile details.
    2. Title this input file as ‘sacinp.*’ where * is the user-defined title. The file contains the model data, member properties defined using Section and Groups. It also contains all the load data, wind areas, Cd, Cm values and Marine growth.
    3. Define the Pile and soil properties are specified separately in the ‘psiinp.*’ file. The soil properties specified are attached from the joints specified as ‘PILEHD’ in fixity in the sacinp file. All soil properties should be defined in the order of axial, end bearing, torsional and lateral stiffness. An initial pile penetration depth needs to be assumed. This has to be specified in the PLGRUP card.
    4. Create the Joint Can check input file called ‘jcninp.*’ where the load cases for which the joint can unity check needs to be performed is specified in this file.
    5. Select ‘Linear Static with PSI Analysis’ option in the Runfile Wizard and select all the above 3 files in the appropriate sections and run the analysis.
    6. The output file ‘psilst’ specifies the pile capacities mobilised versus the capacity required and gives a pile UC ratio value.
    7. Open the ‘psvdb’ folder and check the member UC ratios graphically. The joint can UC ratios need to be checked in the ‘psilst’ file.


    Modal analysis is carried out to determine the various mode shapes of the platform requires the combined Jacket and topsides model to be created in SACS using Preceed-Pro and DataGen modules. The steps are as follows: -

    1. Make a copy of the sacinp file. Rename the new file and make changes in the LDOPT line from NSM to DYN. Further in the LCSEL change the command from ST to DYN.
    2. Specify the retained degrees of freedom as 222000. Normally the corner joints of the jacket and deck are specified as retained DOF’S.
    3. Retain only permanent loads on the structure. Remove all other Load Data. Convert all NGDL weights from Buoyant weights to Dry Weights.
    4. Assuming that superelement is absent take max reactions from the psilst file and create a single pile analysis file called pilinp.* in which these forces are added using the PLSTUB card.
    5. Run single pile analysis and get equivalent pile stub properties .Add these pile stub properties to the sacinp file along with its group and section properties.
    6. Create dyninp file and specify number of modes to be extracted.
    7. With the modified sacinp and the dyninp file run a analysis in extract mode shapes and check dynlst file for frequency and mass participation factor. This factor should be 95% at least.


    1. Make a copy of the inplace sacinp file. Rename the file as sacinp.fatigue.
    2. Make following changes to this file:
    a) In the LDOPT card change the Water Depth as per bid to account for absence of Storm Surge

    b) Change the Cd and Cm values

    c) Delete all loads except wave loads

    d) Change the Kinematic factor to 1.0(see bid) in the WAVE card

    e) In the Wave Height field, change the wave height to Average wave height of the specific wave

    f) Enter MS for obtaining maximumbase shear value

    g) Delete all Load combinations from this file.

    h) Advance the wave in steps of 4degrees

    i) The number of static steps will therefore be 360/4 = 90

    1. Run this file in Static Linear static analysis Select sacinp.fatigue*
    2. In the output listing a saclst file is obtained from which the crest positions for minimum and maximum shear can be found for different wave heights and different wave directions.
    3. Obtain three angles between angle1(X) and angle 2(Y) as (Y-X)/4 and remaining three angles as ((360-Y)+X)/4
    4. Enter the 6+2 angles in the sacinp file and change the number of steps to1 in increments of 1degree.
    5. Run the sacinp file in Linear Static Analysis.
    6. A saccsf file is obtained which will be used for the fatigue analysis.
    7. Create a ftginp.* file.
    8. In the FTOPT card enter design life(see bid) and factor(see bid, usually 2.0). Also enter the fatigue time period as the Wave Period (generally 1 year).
    9. Initially apply API X Prime for source of S-N curve i.e. APP.
    10. For SCF’s use Kuang & Wordsworth for all joints initially.
    11. In the FTOPT2 card give PT, Export Fatigue data, Tubular Inline Check, Inline Tubular SCF-AWS, and Effective Thickness Ratio-2WAL
    12. Specify the SCF limits in the SCFLM card as a maximum of 6.0 and a minimum of 1.6
    13. For Grouted Joints enter Joint Override with SCF Option as Marshalls Method.
    14. In the GRPSEL RM card specify dummy structures, appurtenances, Risers and conductors which are not part of the main structural Member but attract Wave Load.
    15. In the EXTRAC HEAD AE card enter a cut off of 0.5 to extract joints which have a fatigue life of less than 50 years.
    16. Now, in the Runfile Wizard go to Post Fatigue Damage and Run the ftginp file with the saccsf file and note down the joints which have service life of less than 50 years.
    17. Now, Extract these joints individually by using the EXTRAC card in the ftginp file.
    18. On running the file again as in step no.18, a ftgext file is created automatically.
    19. In the ftgext file we can make changes in the Chord Thickness, or S-N curve to be used etc. to find the optimum change that has to be made to a chord/brace. Note down the specific changes that need to be made for a specific joint.
    20. Now, in the ftginp file enter the JNTOVR cards for the joint overrides that need to be specified as noted from the ftgext file.
      NOTE: In the case of grouted joints, if the S-N curve needs to be changed, use the API X curve with effective thickness option i.e. AXP option.
    21. Run the Final ftginp file with the saccsf file till no joint have a service life
      less than 50years.
    22. The output files that are obtained from the run are the ftglst and the ftgext files.


    1. Create 5 directories under seismic analysis folder – Static, Pile, NatFreq, Earthqk and Post.
    2. In Static folder, run a Linear Static analysis with PSI option for the In-place model.
    3. From the ‘psilst’ file obtain the max. axial, lateral forces and moment for any pile group and the axial displacement from operating storm load cases only.
    4. In Pile folder, Make a copy of the psiinp.* file and rename it as pilinp.*. In the datagen of the pilinp.* change the PSIOPT to PLOPT. At the end of the soil data, add PLSTUB card with the force values obtained in Step 3 above. (Note: Retain the soil prop. and a single pile group in the file, copied from the PSI input file).
    5. Run Single Pile analysis ( In MISC in Runfile Wizard) and from the ‘pillst’ get the pile stub dimensions. Update the Inplace model by removing the pile group members and pilehead joints and adding the pile stubs instead to it. Also paste the pile stub section property line to the input file.
    6. Copy the input (sacinp) file generated in Step 5 above to the NatFreq directory. Make all corner nodes of the various levels as ‘222000’. Delete all load cases except one combination for operating loads with suitable contingencies. This load case should not contain any environmental load data. Name it ‘SLE’ and ‘DLE’ for Strength Level and Ductility Level Earthquake runs respectively. Include DYN option in LDOPT card and DY in LCSEL card.
    7. Create a ‘dyninp’ file with the number of mode shapes. Specify SA option in DYNOPT card and run a Dynpac analysis. Open the output file and check the period and total mass participation factors.
    8. Copy the input file generated in Step 5 above to the Static directory. Add LCSEL card with load case ‘SLE’ or ‘DLE’ and specify ‘CMB’ option in the LDOPT card. Run a Linear static analysis.
    9. Copy the updated model, the ‘dynmas’ and ‘dynmod’ files generated in Step 7 above to the Earthqk directory. Copy the ‘saccsf’ file generated in Step 8 above to the Earthqk directory.
    10. Create a ‘dyrinp’ file specifying SLE as the primary load case in the STCMB card and a factor of 2.0 for Joint can check.
    11. Run an earthquake analysis with the above files and generate the ‘dyrcsf’ file. Check the max. axial, lateral forces and moment under the ‘CQC SUMMATION FROM ALL DIRECTIONS’ column in the ‘dyrlst’ file.
    12. These should be compared with the values added in Step 4. In case it is different, update the ‘pilinp’ file with these values.
    13. Repeat Steps 5 to 12 till the values converge to a reasonable limit.
    14. Create a ‘pstinp’ file in the Post folder. Select Load Case 1 and 2 only i.e., {Earthquake+ Static (Tension)} and {Earthquake + Static (Compression)} with a AMOD of 1.7 on the allowables.
    15. Perform Element Code check and generate a Postvue Database file using the ‘dyrcsf’ file generated in Step 11 above.
    16. Create a ‘jcninp’ file with AMOD as 1.7 for Load Cases 3 and 4 only i.e., {Earthquake + Static (Tension)} and {Earthquake + Static (Compression)} for joint check case. Run Joint Can analysis.


    1. The steps 1 to 9 specified in the Seismic Analysis section 5.0 above have to be first performed in the vibration analysis run.
    2. Note : Retain relevant degrees of freedom including nodes present on equipment.
    3. Create a dyrinp file and specify the run speeds of the reciprocating machines in the RSPEED card. Change the number of modes in the ENGVB card. Specify the unbalanced force and moments acting at various joints of the structure using the UNBAL card. The damping factor is 2% .
    4. Run a dynamic response analysis using the dyrinp and the dynmas and dynmod files generated from the modal analysis steps.
    5. Check the displacement levels in the joints versus the allowable specified in the dyrinp file.
    6. In case the displacement is more than the specified value for some joint provide minor plate stiffening in the sacinp file and re-run all steps.
    7. Make sure that enough mode shapes are extracted to cover the engine running speeds by 10% extra at least so that any resonance is picked up in the analysis.
    hoangtu thích bài này.

Chia sẻ trang này