November 8, 2018 at 9:55 pmnavidzSubscriber
So I have some confusions about the hydrostatic elements (HSFLD241 or HSFLD242). I understand that these elements have displacement DOF and an extra node that take care of the pressure DOF and by defining the location of the pressure node we can have positive or negative volume (or area for 241). So the first thing that I do not understand is the use of positive and negative volume. Is it only to say that there is mass in the positive volume and no mass in negative volume or does this + or - volume can change the pressure distribution. Let me explain my problem to make it more clear.
I have a simple cubic domain that has a spherical cavity inside it. In reality, this spherical cavity is filled with water which is incompressible but because I do not want to link my static structural modeling to fluent, I used HSFLD242 elements that are designed for this type of situation. Since the volume of the sphere is very small, I do not care about pressure change as we go more inside the fluid. So the pressure is completely uniform in the sphere. I also do not want to give initial pressure to the water. Now the solid domain deforms (large deformation) and due to that, the sphere will deform to something like an ellipsoid. Do I need to care about the + or - volume of the HSFLD242 elements (especially that I chose keypoint(5)=0 for HSFLD242 which means that there is no mass of fluid)? can this strategy accompany with keypoint(6)=1 capture a physics that volume is not changing but the pressure of the fluid will change?
So my main issue is that my geometry is not simply a sphere and it is a convex geometry as I mentioned in:
So there is no way that I can simply define my HSFLD242 elements with only one fluid pressure node and get positive volume everywhere. So I am wondering if the + or - volume matters or not for this problem. If it matters, how can I use HSFLD242 for a convex geometry while we now that there exist fluid everywhere in the cavity even if the volume goes out of the cavity?
November 19, 2018 at 4:09 pmnavidzSubscriber
So does HSFLD242 work for convex 3d shapes?
November 21, 2018 at 12:40 amBhargava SistaAnsys Employee
The negative volume is useful when the pressure node is located outside the fluid volume. In such cases, the volume of the fluid elements will be more than the volume of the actual fluid domain which is why a negative volume is needed to compensate for that extra volume. Since the fluid material models are governed by the relation between pressure-volume, the negative volume compensation is necessary for such case. A very good example for such cases is the inflated tire, as you can imagine the location of pressure node will be outside the tire volume so the volume correction is important. (check out this link: https://ansyshelp.ansys.com/account/secured?returnurl=/Views/Secured/corp/v192/ans_str/strhydrodefine.html)
Coming to your problem, the fluid domain in your case is the two spherical voids and the channel connecting them. When you pick the entire volume as one, the pressure node will be placed somewhere inside the channel. This case is similar to the inflated tire example, a portion of the volume calculation will fall outside the fluid region so negative volume elements are introduced to compensate for it. I'd recommend that you proceed with this setup, watch out for the negative volume messages (you should get them) and finally take the model into MAPDL and plot the fluid elements to visually verify how the volume elements are connected to the pressure node.
November 21, 2018 at 4:26 pmSandeep MedikondaAnsys Employee
In addition to what Bhargava says above. I wanted to point you out to this example from the Technology Demonstration Guide.
I've talked to a colleague with expertise in this and according to him:
"Some elements may have negative volume, others positive volume and this is just fine. It is in fact (I believe) the way these elements are supposed to work"
Also, these are not natively exposed in mechanical are you using an extension or MAPDL?
November 21, 2018 at 4:41 pmnavidzSubscriber
Thanks, Sandeep and Bhargava for your through explanations. So as far as I understand it does not matter whether the geometry is convex or not. In fact, it might have some negative volume elements that are there to incorporate for higher occupied volume.
I am using the following code that to get the plot of elements and pressure of the HSFLD242 elements from Workbench.
/show,png ! output to png format
/gfile,650 ! adjust size of file
/edge,1,1 ! turn on element outlines
/view,,0,0,1 ! adjust view angle
*get,my_pres,node,newnode,hdsp ! ewnode is the name of the pressure node
April 9, 2020 at 2:05 amyy4g17Subscriber
Hi, sorry for the very late reply, for the project I am currently involved in, I have to model tyre deflection characteristics with presence of inflation pressure, I am trying to use HSFLD242 element to achieve this, but how do I apply this element in WORKBENCH exactly? I dont have lots of experience with APDL commands...Thanks!
- You must be logged in to reply to this topic.
Earth Rescue – An Ansys Online Series
The climate crisis is here. But so is the human ingenuity to fight it. Earth Rescue reveals what visionary companies are doing today to engineer radical new ideas in the fight against climate change. Click here to watch the first episode.
Subscribe to the Ansys Blog to get great new content about the power of simulation delivered right to your email on a weekly basis. With content from Ansys experts, partners and customers you will learn about product development advances, thought leadership and trends and tips to better use Ansys tools. Sign up here.
- Saving & sharing of Working project files in .wbpz format
- An Unknown error occurred during solution. Check the Solver Output…..
- Understanding Force Convergence Solution Output
- Solver Pivot Warning in Beam Element Model
- Colors and Mesh Display
- How to calculate the residual stress on a coating by Vickers indentation?
- whether have the difference between using contact and target bodies
- What is the difference between bonded contact region and fixed joint
- The solver engine was unable to converge on a solution for the nonlinear problem as constrained.
- User manual
© 2023 Copyright ANSYS, Inc. All rights reserved.