23 November 2018
- Last edited 23 November 2018
Hello Siva Teja,
Regarding your first question, "But we can give the pressure distribution at only one time-step as can be seen in the next picture..."
- Simply add the new data (new Pressure file) in a new row. You can change the analysis time accordingly (also scale or offset if needed) as shown in the image below.
Regarding your second question, "But, when I tried to solve with this loading and check the "Imported pressure" under the "Solution" tree, it is showing that the max. and min. pressures to be "0". Is it because of the warnings that are being shown at the bottom... (picture attached)"
- Honestly speaking, I am not sure how you got this post-processing object, for Imported Pressure. Please clarify the steps you used to get this.
In any case, if you want to plot the imported pressure, you can do it via User defined result, by plotting SMISC13 values on the SURF154 elements created due to the applied pressure load.
1. Set, General Miscellaneous --> Yes (under Analysis Settings --> Output Controls --> General Miscellaneous). This is to store the miscellaneous results, while, SMISC13 comes under this category.
2. After solution, click on Solution branch in the tree, then toggle on Worksheet. Here you can select "Material and Element Type Information", after which you can simply RMB on SURF154 in this table --> Insert User Defined Result. (If you have multiple SURF154 types, RMB --> plot items helps you understand which of them corresponds to a particular load you are interested in). Then in the User defined result, provide under Expression, SMISC13. This will evaluate the applied pressures.
Hope this helps. Let me know if you have any questions.