Hi guys! I want to parametrize a quantity (take velocity) but the velocity here is not constant value, instead it is different at different time steps (tabular data). As soon as I put tabular value for velocity the box to click for parametric disappears. How do I parametrize it?
How to parametrize tabular data?
- 41 Views
- Last Post 4 weeks ago
Unfortunately, it is not possible currently to parametrize a tabular boundary condition (say Velocity) in Mechanical.
The workaround is to define the velocity table and the velocity boundary condition via APDL commands in a Command object (under Transient Structural). Command objects have input arguments which can be parametrized (Arg1, Arg2...). You can use these Arguments to input velocity values in the defined table.
Regarding creating table and defining values, you can have a look into the input file (click on Solution --> Tools --> Write Input file), and copy the APDL commands corresponding to the GUI definition of Velocity table and paste it in the Command object (suppress the GUI velocity object) and modify the commands as per your need.
Please give this a shot and let me know if you have any questions. All the APDL commands are documented in ANSYS help if you want further reference.
But the issue with this is the maximum number of arguments is 9. If we have 60 load steps with 60 velocities to parametrize, what can be done?
I don't know if this will help you. I got help from a talented support engineer at SimuTech Group. Below is a description of what he created for me.
I had a Transient Structural model that had tabular input for the Acceleration load which varied over time. There was only one load step. The time history was very large, 42,000 time steps with three values per step (xyz), which is 126,000 numbers. Workbench almost chokes on this many numbers and takes forever to submit to the solver.
Instead, I put the 126,000 numbers in a text file, and used a command snippet to read the text file.
The load now just has three numbers, 1, 1, 1 for xyz accelerations.
The command snippet is this:
! Commands inserted into this file will be executed just prior to the ANSYS SOLVE command. ! These commands may supersede command settings set by Workbench. ! Active UNIT system in Workbench when this object was created: Metric (mm, kg, N, s, mV, mA) ! NOTE: Any data that requires units (such as mass) is assumed to be in the consistent solver unit system. ! See Solving Units in the help system for more information. /input, E:\Excel\ansys\accel.txt lvscale,%_acelx%,1 lvscale,%_acely%,2 lvscale,%_acelz%,3
and the text file looks like this:
*DIM,_acelx,TABLE,42000,1,1,TIME, ! Time values _acelx(1,0,1) = 0. _acelx(2,0,1) = 7.14286e-004 _acelx(3,0,1) = 1.42857e-003 _acelx(4,0,1) = 2.14286e-003 _acelx(5,0,1) = 2.85714e-003
... lots more rows of data ...
_acelz(41995,1,1) = 9782.35101 _acelz(41996,1,1) = 9785.600918 _acelz(41997,1,1) = 9789.241912 _acelz(41998,1,1) = 9793.198973 _acelz(41999,1,1) = 9797.390961 _acelz(42000,1,1) = 9801.731686
The text file was created by writing out the input file once using the agonizingly slow Workbench and finding this section for the text file.
- 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