I want to apply acceleration on a solid steel beam. After using Kobe earthquake data for 16 seconds, the deformation varies until 2.5 seconds and after that it is constant. what is the solution to it? and what is the concept behind initial time step, minimum time step and maximum time step?
time history analysis
- 134 Views
- Last Post 4 weeks ago
- Topic Is Solved
1. What is the first natural frequency of the solid steel beam?
2. What is the highest mode shape you want to include in the results? What is the modal frequency of mode 3?
The guidance for Transient simulations is to have 20 time steps within the highest frequency of interest. So if mode 3 was 30 Hz, then the sampling frequency should be 20x30 = 600 Hz and that means a time step of 1/600 seconds. That should be the initial time step and the maximum time step. The minimum time step can be 10 times smaller.
Hi Peteroznewman, thank you for you reply.
Can you please help me out with the attached problem.
You won't get good results with a solid tet mesh that looks like this.
Convert your geometry to either a midsurface model or a beam model and come back when you have done that.
Midsurface means you will have three surfaces at the center of those walls. In Mechanical you will assign the wall thickness. The flanges will have a split in the face where the web attaches in the center.
Beam model means click on Extract in the Beam tools on the Prepare tab in SpaceClaim and you will have beam elements in Mechanical with the cross-sectional properties of the I-beam automatically created.
I tried doing with beam model but in that case I am not able apply support in the lower flange edge as the edge is not getting selected.
In a beam model, the vertex at the end represents the entire cross-section. The vertex can be Fixed (no rotation) at one end and Pinned (rotation allowed) at the other end.
thank you for you prompt response sir. Kindly check the transient analysis settings in the problem and let me know any changes that I should make.
And can you clarify through images about how supports can be applied?
Here are the Fixed Support and Displacements from your model reassigned to the vertex at each end of the line body.
Here is the displacement support.
Make sure you have the Geometry filter set to Vertex.
Once you have that, add a Modal analysis and Solve that to answer my questions on the natural frequencies.
Note that you drag and drop the Fixed Support and Displacement into the Modal Analysis.
Now Drag and Drop a Transient Structural and drop it on the Solution cell of Modal. Then drag the Acceleration load from the first Transient Structural onto the last Transient Structural.
The last Transient Structural is the Modal Superposition Method.
If i want to make perforations in the web part of the beam, then how am I supposed to that??
Since you can create the solid I-beam in SpaceClaim, you already know everything you need to create the surface model I-beam. Draw three lines and Pull them to the length of the I-beam. Optionally, you can project the center web onto each flange to split the face, but you can connect the web to the flange in Meshing.
The Fixed Support is understood what that means. What exactly do you mean with the displacement support? Do you mean that the full boundary of the cross-section is prevented from moving in X and Y, and is therefore not free to rotate about Z? Or do you mean the end is captured by a pin that prevents X and Y motion, but allows the cross-section to rotate about Z?
Where did you get your Kobe earthquake data? I went to this website and found that at one station,
the magnitude of the peak acceleration was 0.82 g = -8.05 m/sec/sec = -805 cm/sec/sec = -8050 mm/sec/sec
Your data shows a peak magnitude of - 8.05 mm/sec/sec. Do you think you are off by a factor of 1000???
Yes, actually I forgot to change the unit of earthquake data.. thank you for rectifying me out. I want to create a simply supported beam, so after some web searching and videos I found out that providing fixed support at one edge and displacement at another ( in which movement is restricted in X & Y direction and free in Z direction) will give same result as simply supported beam.
and in surface I beam model, if I only work on three lines then when should I provide the thickness to flange and web?
Yes, you assign a thickness to the surfaces in Mechanical. If you use the Midsurface feature in SpaceClaim, it does that automatically.
The support conditions for simply supported beam mentioned in the previous comment makes any sense or not?
Kindly check the attached mid surfacing. Is it giving proper result?
The center web is not connected to the flanges. You can tell because of the red color in the Mesh display.
You can fix that by right click on the Mesh branch and inserting a Mesh Connection Group, then right click on the Mesh Connection Group and Detect Connections, then Generate on the Mesh. Now the web is connected to the flanges as shown by the color purple.
I thought the Fixed Support might include all 5 edges, you only have two edges selected. Is that because it is only connected at the bottom flange? If so, then that is fine. Same question for the Displacement at the other end and I see that it is only supported in Y so is free in both X and Z which means it is like having a plate on spheres.
The Analysis should be set up as a two step Analysis. Step 1 is for gravity to take effect so turn Time Integration Off and zero the values of acceleration up to time 1 second. Then Step 2 has Time Integration On and tracks the deformations on the already deflected beam. If you don't do that then you are suddenly applying gravity at time zero and that does not represent reality.
Another observation is that the earthquake data you have is for lateral earth motion, while you have assigned it to a vertical motion. I suggest you copy the data out of the Y column and paste it into the X column. I did that and copied the zeros out of the Z column to put in the Y column, but in reality, the ground motion had X, Y and Z data so you could have put all three in the acceleration load, but the Z would have almost no affect as it is along the axis of the beam.
Finally, to make the result more interesting, under Geometry, you can Insert a Distributed Mass and assign 1000 kg to the web face.
I am working on the changes you have suggested. What according to you should be the support conditions for this beam to behave as simply supported? and can you help me out with the procedure for two step analysis?
I did the changes that you suggested. Kindly check the attached file and just clear my doubt of support condition. And thank you so much for your patience in clearing my doubts.
I have one doubt, suppose I open static structural module and apply line pressure on a beam and then link transient structure module with static structure and apply acceleration over the beam. Then will the line pressure get overlap in transient structure module as well?
- All Categories
- Community Rules, Guidelines, and Tips
- News & Announcements
- Student Products
- Pre and Post Processing
- Physics Simulation
- Tutorials, Articles and Textbooks
- Installation and Licensing
- Student Competition Teams
- eMasters Degree from UPM
- Site Feedback