Real Time Simulation of a Force impact on Blade
- 60 Views
- Last Post 31 May 2020
Keep this discussion, but delete the one below since it seems to be a duplicate.
Please advice on my problem questions? please.
I deleted the Post
In Workbench (WB), drag out a Modal Analysis. Right click on Geometry and Edit in DesignModeler (DM). In DM, File > Import External Geometry File. Create a Plane that goes through the blade at some distance x from the tip. Use that plane to Slice the body into two bodies. In the Outline, select the two bodies, right mouse click and Form New Part. That has made a multibody part. Now you have a face between the tip of the blade and the plane to apply a force. This takes care of the Dirac delta function. Force on one face, no force on the adjacent face. Later you can create a Parameter to move that plane up and down along the length of the blade. Close DM.
In WB, drag out a Harmonic Response and drop it on the Solution cell of the Modal analysis. Double click on Model cell of the Modal analysis. In Mechanical, under the Modal section of the outline, select the faces at the root of the blade and assign them as Fixed Support. Solve the Modal analysis. Look at the range of frequencies. Create some Deformation plots to look at the mode shapes. Animate them.
In Mechanical, under the Harmonic Response section of the outline, select the face at the tip of the blade and assign a Force. The value you type is f0. The analysis will automatically apply this as a harmonic load with a sinusoidal variation.
Under Analysis Settings set the frequency range minimum and maximum values and the number of Solution Intervals. Under the Damping Controls section, set the Damping Ratio. Under the Solution branch of Harmonic Response, insert a Frequency Response and select a vertex at the tip of the blade and assign a direction that is in line with the maximum bending mode.
I forgot to mention that you must go into Engineering Data, and add the material of the blade. Minimum properties are Density and Isotopic Linear Elasticity, which needs just the Young's Modulus and Poisson's Ratio. Then in Mechanical, under Geometry, pick the two solid bodies and assign that material.
So my first approach using static structural is not a fit to this example.
What if I want just to apply it on one point not a plane just one point like in the example below. a transversal force on a point to the tip of the Blade?
If you make a plane at that height and slice the body you will have a horizontal edge you could apply. That should be good enough.
If you make a vertical plane through this point to slice the body into 4 pieces, now you will have a vertex at that point.
Thank you so much,I will keep it open I will just follow your guidelines, I will mark it as solved at a later stage to avoid repetition and all since I think I will need more help at some steps
- All Categories
- Community Rules, Guidelines, and Tips
- News & Announcements
- Student Products
- Pre and Post Processing
- Tutorials, Articles and Textbooks
- Installation and Licensing
- Physics Simulation
- Student Competition Teams
- eMasters Degree from UPM
- Site Feedback