Simple Modelling using SACS

Lets begin SACSing!!!


Using SACS is (somehow) not as hard as it seem. We are going to learn by directly modeling this basic structure. This tutorial uses SACS-EDI v5.3

simple model

The first window shown by SACS 5.3 is what I called the Program Manager. Why so? (because i like the name) Seriously, it’s simply because we have many options inside this window, from modeling, run analysis, view result, etc. Three (of many important) parts in this program manager are:

program manager

  • Program Launcher (located on the very left of the window), where we choose what we are going to do:
    • Modeler, launch PRECEDE which we use to model the structure
    • Data File, launch DATAGEN which we use to create the model in text ways, or create run file (e.g. input for seastate analysis, input for combine file, etc.)
    • View Results, shows the result in model-view (normally the extension is psvdb)
    • Some more.

folders

  • Folderswhere we put our works into. It is important to work inside a specific folder. Using folder will make our works tidier. For example: an FPSO project normally has many analyses (e.g. in service, fire, transit, fatigue, and many more), hence each folder for each analysis.

In in-service analysis, I usually use 3 steps. First step is set-down, so one folder for it. Followed by sea-state step, where we have inertia force (by wave, wind, etc.), so it’s another folder. Also a combining folder to combine the set-down stage and sea-state step. We can manage our work, by doing folder inside folder. It will make us follow the steps, thus minimize the risk of my human error. For example this is a print screen of some analysis.


  • Run-Analysis and Inside folder windows, the last windows in the right side is where we choose the analysis.

1. Start Modeler, SACS PRECEDE windows will come out. Choose blank model, with metric kN unit.

SACS analysis is based on finite element; hence the use of joint is obligatory. Not like other structure aided program, where line option will automatically add the two joint at the start and the end of line, the SACS program is rely on the joint we create first.

2.Choose Joint – Add – Absolute

Joint name consists of 4 characters. The program can create the name automatically, but we can (as always) override the joint name. Input as follows:

Joint Name
X
Y
Z
0001
0
0
0
0002
6
0
0
0003
6
6
0
0004
0
6
0
0005
0
0
6
0006
6
0
6
0007
6
6
6
0008
0
6
6

Let the fixity option blank, we will return to it later.

3.Choose Member – Add

Member should be labeled with 3 characters. For example B01, which refers to beam number 1; or B1x, which refers to beam at level 1 and x-specification (e.g. tubular, I-beam, etc.). There is always the good and the bad side of these kinds of naming.

   
+ Structural properties can be modified one by one (for example beam in the same level has different properties) + Modeling is simpler, since we don’t define to many beam properties
- We must define each of structural member’s properties - If somehow the model should be changed. All the corresponding structural members change also.

For this example,

Member Group Label
Joint Number
B1I
0005
0006
0006
0007
0007
0008
0008
0005
C1T
0001
0005
0002
0006
0003
0007
0004
0008

You can either enter the joint number one by one, or select the joint directly in the model.

Ps. To show the number of joint, click the joint symbol  on the toolbar to show joint name.

4.To create brace member, click joint – add – relative.

Ps. you can either enter the join name manually or let SACS create it automatically. If the joint name you entered already exists in the model, it will show warning (there's also an option to select the subsequent number)

There are 8 bracing (as shown in the figure). Thus, we create 12 new joint (it has the same distance of 1.5m).

5.Add brace member, click member – add

For this example, name the bracing group label with BR1

6.Add member section, click property – member section

Create wide flange beam with properties as follows:

  • Width of beam= 20 cm
  • Height of beam= 50 cm
  • Flange thickness= 1.6cm
  • Web thickness= 1 cm

Ps. we can also override the properties of our member by defining manually the axial area, torsional moment of inertia, and moment inertia (strong or weak axis) - but not in this case.

Ps2. we only define the I-member. For the tubular member, we will define it directly in the member group (the following).

7.Add member properties, click property – member group

  • In Section label click “”, and choose I5020. You can also edit the dimension by click Edit.
  • Modulus young (E) of steel is normally 2e5 MPa. The shear modulus (G) is given by :

Where the poisson's ratio (Ʋ) of steel is normally 0.3, Thus G would be 76923.08 MPa. We use the yield stress (Fy) of 358 MPa and the density of 7849 kg/m3.

  • Some other options, (but we don't need them in this tutorial)
    • Segment, in my opinion is when we have welding connection or segmented part. For example, we have span of 8 m. Normally the length of member is 6m, so we could either design 6m and 2m or 4m each. If we use segment, we could define the length of segment and/or increase the yield strength of the segment (since the weld yielding stress is as great as 458 MPa for E70).
    • Flooded member affects the hoop force calculation for hollow section, (e.g. tubular or pipe member), also calculation for buoyancy forces.
    • Tensile strength is used when we have plastic analysis. Tensile strength is the same as ultimate strength where the member is failed (rupture).

For BR1 and I1T, we will enter the member group properties without entering the member section properties first. This option not only allows us to create the model quicker but also the ability to define the member shear area.

Member Group
Outside Diameter (cm)
Thickness (cm)
Yield Stress (MPa)
BR1
13.2
1.1
358
I1T
30
2.5
358

By default SACS defines the shear area to be 0.5 (either API or ISO code use 0.5 as shear area coefficient). Though, you can override this value by clicking miscellaneous.

After defining all member properties, the member group manager will look like this:

8.Add loading.

Suppose that there is a plate which we can neglect its weight. The weights are:

  • Imposed dead load: 1.5 ton/m2
  • Live load: 0.75 ton/m2
  • Variable load: 1 ton/m2

To distribute the loading, we must calculate it manually first. The loads can be distributed either by envelope method or one-way-slab method. Since we have the ratio of length and width of 1 (less than 2.5), envelope method is used.

Using standard envelope of 45º angle, we have the center of envelope at (3,3).

Type of Loading
Area (m2)
Loading (tonne/m2)
Total load (ton)
Member Load (ton/m)
Imposed DL (Load Condition 2)
36
1.5
54
2.25
Live Load (Load Condition 3)
36
0.75
27
1.125
Variable Load (Load Condition 4)
36
1
36
1.5
  • Click Load – Member

  • Select the corresponding member, and then input the load condition, load ID, load ID filter (optional). The load type we use is force, in global Z coordinate. Input the corresponding load value (initial and final).
  • To check, whether if we have already define the loading or not, click Load – Display/Modify

9.Add Self-Weight, by clicking Load – Self Weight

Input as follows:

  • Load condition: 1
  • Load ID: Dead
  • Load direction: -Z
  • Acceleration (G): 1 (it’s mean 1 gravity or 9.81 m/s2)
  • Load disposition: Add

10. Create load combination.

Based on ISO code, we will create one load combination for dead load, live load, and variable load. Click Load – Combine Load Conditions

  • Load combination: 100
  • Combination: 1.3 DL + 1.3 IMPS + 1.5 LL + 1.5 VL

11.Don’t forget the boundary condition or in this case Joint Fixities. Click Joint – Fixities.

Click joint (using ctrl) 0001 – 0002 – 0003 – 0004 and choose 111000 (pinned condition).

SACS uses 6 degrees of freedom, and its fix X-Y-Z-Mx-My-Mz.

Voila, the final model

Save your work inside of folder (e.g. Desktop/Training/sacinp.model1)

Running Analysis

Go back to SACS program manager and find our last training folder, click the folder, hence we are working inside the folder.

  • Choose Analysis Generator

  • Use Static Analysis – Basic with Solve options only. Choose your sacs model file and name the output and listing files as your wish.

  • Click Run Analysis

THERE WILL BE ERRORS (LOTS OF)

Why?? Because SACS depends on joint, especially 2 joints for 1 member.

  • Go back to Files and use “drag and drop” method for sacinp.model1

The problem of our model is a member having more than 2 joint. The column has 3 joints, since there is an added point for bracing modeling (Even the beam has 4 joints :p).

  • To fix this model, click Member – Divide – Existing Joint. Choose the entire related member that has more than 2 joints for 1 member.

  • Finish for all the troubling members and save the job.
  • Re-run the analysis by clicking “sacmodel1.runx”


This is the end of the tutorial

next we will learn analyzing the results


4 Responses to Simple Modelling using SACS

  1. Vikas says:

    Great !!
    Simplified the modelling !! Great!!

    • marcieladewa says:

      hey, thank you for visiting my blog

      unfortunately i haven’t yet uploading the pictures which are included normally. I will get them uploaded as soon as i get a good internet connection

      thank you once again.

  2. Hendi says:

    Good Job Bro… Keep Posting.. I have Sacs v5.3…

    I want to learn more.. even not related to my job now… wkwkwkw

    Input : could you add some picture.. hehehehe…

Leave a Reply

Fill in your details below or click an icon to log in:

WordPress.com Logo

You are commenting using your WordPress.com account. Log Out / Change )

Twitter picture

You are commenting using your Twitter account. Log Out / Change )

Facebook photo

You are commenting using your Facebook account. Log Out / Change )

Google+ photo

You are commenting using your Google+ account. Log Out / Change )

Connecting to %s

Follow

Get every new post delivered to your Inbox.

%d bloggers like this: