Comparing results computed in 3d models in 2 different meshes/points in paraview

[Sajeda Akter]

Hello Simvascular developers,
I am using Simvascular for coronary blood flow simulations. After simulation I received .vtu, .vtp and some other files. I have some questions regarding the post-processing:
1) I would like to ask that how can I compute the values in 2 different meshes/points e.g. for FFR value, I need upstream and downstream records of stenosis of the simulated model using paraview.
2) In my simulated model, how can I see the velocity (vector) magnitude and streamlines in 3D paraview layout?

Thanks in advance

Best.
Sajeda

[Justin Tran]

Hi Sajeda,

Thank you for your question and interest in SimVascular! To look at computed values at certain points in your simulation results, we recommend using the "Clip" and "Slice" filters. These filters will allow you to define a plane (or box, or cylinder) with which you can cut through your model. You can then examine the computed values in the resulting slice. You may also find it useful to quickly examine computed values at specified points in your results. You can do this with the "Hover Points" feature. To turn on Hover Points, you will need to click the button with a "?", which is located above the 3D display and below the common filters toolbar. With this on, if you hover your mouse over a mesh point in the 3D display, it will show the value of the currently selected variable. Another useful tool is the "Integrate Variables" filter. You can integrate all the variables of interest and divide by the area or volume to get an average value of that variable in a region. Using "Integrate Variables" is particularly useful after performing a slice in the case that you want to compute an area-averaged pressure in a sliced cross-section.

You can view the velocity magnitude by displaying the velocity field variable. You can select velocity from the "Active Variables" toolbar. Though if you display the velocity field on a rigid simulation result, you will likely see 0 velocity across the entire model (since the rigid wall assumption forces the velocity to zero at the walls). In this case, we recommend slicing through the model in your area of interest, then displaying the velocity magnitude.

You can display streamlines by using the "Stream Tracer" filter (selectable from the "Filters" menu at the very top). Upon selecting this filter, you will be asked to place a "seed" point, from which the streamlines will start by mousing over a point in your model and hitting "P" on the keyboard. You can then use the "Properties" tab on the left to select the size of this seed, length of the associated streamline, and number of streamlines to display. Then, hit "Apply" and your streamlines should be displayed at that point. Feel free to tinker with the settings to get the right density of streamlines that you desire.

Hope that helped! Let us know if anything is unclear or if you would like more tips on postprocessing in Paraview.

[Sajeda Akter]

Thank you very much Justin for your elaborate and rapid reply. I hope that is helpful.

I have one more question that for velocity magnitude slicing filter give horizontal result but I want to see velocity condition in whole model e.g. I have C type RCA model. How can I see velocity condition in this way?

Thanks again. I think you are very helpful.

Regards,
Sajeda

[Justin Tran]

Hi Sajeda,

To view the velocity magnitude for the whole model, you can try the Volume Rendering option. By default, Paraview displays model in "Surface" mode, which only shows the calculated variables on the surface of the model. You can confirm this by observing that the option for "Surface" is selected from the display drop-down menu, which is to the right of the active variable selection menu near the top of the screen. You can then select "Volume" from this drop-down menu and you should see your model turn into kind of a gas cloud, with the colors representing the magnitudes of your variable of choice. Change the variable to the velocity, and you should be able to see a volume rendering of the velocity field throughout your model.

Alternatively, you can color the stream lines by the velocity magnitude. After creating streamlines using the "Stream Tracer" filter from last time, you can again change the active variable at the top of the screen to velocity. This will color your streamlines by the magnitude of the velocity vector. This is a convenient way to show both the magnitude and direction of velocity vectors inside your model.

Hope that helps!

[Sajeda Akter]

Thank you Justin...you are really helpful.

I am stack in another question that vWSS. When I saw in hover point then vWSS like as a coordinate but in line bar its range e.g. 0 to 50...therefore, how can I take a number from hover point like as pressure?

Thanks

[Justin Tran]

Hi Sajeda,

I think it is likely you are viewing the magnitude of the vWSS vector in the line bar. But when you hover over the points, you are looking at the (x,y,z) coordinates of the vWSS vector. One way to display the magnitude of the vWSS in hover points is to create a new array which computes the magnitude of the vWSS vector.

You can do this with the "Calculator" filter. Click the button in the top left that looks like a calculator to open the Properties tab of the Calculator filter. You should see a grid of possible operations (i.e. sin, norm, ln, etc.). We want to use the "mag" operation for the magnitude. Click this, and you should see "mag" appear in the text line above the grid. Then, click the button for the open parenthesis "(". Then, click the "Vector" drop-down menu below the grid of buttons and select vWSS as your vector. You can then rename this new array by changing the text "Result Array Name". Click "Apply", and this should create your new vWSS magnitude array.

Now, when you do Hover Points, you should be able to see your newly computed vWSS magnitude.

Hope that helps!

[Sajeda Akter]

Thank you very much and I hope you all are fine...although I am late.

I have one more question that is there any tool or technique in simvascular or paraview or else to measure the length of a path or 3d model and measure the areas of inlet and outlet of a 3D model.

Thanks in advance...

[Justin Tran]

Hi Sajeda,

Glad that helped! Measuring the length of a path is difficult. I usually accomplish this task using Python VTK scripts.

Measuring the area of inlets and outlets is built into SimVascular! If you click and highlight a face in the Modeling tab, on the bottom right of the screen you should see a little tooltip which shows the area of that face.

Hope that helps!

[Sajeda Akter]

Thank you very much Justin...I hope it will be work....you are very helpful

[Sajeda Akter]

Hello..
I hope you all are fine...
Could you please give some suggestions or instructions me that why simulation results glyph vector orientations (in paraview) opposite i.e. its look flow from outlet to inlet...but I input inlet velocity profile parabolic and steady state...Moreover, I also see average pressure and pressure are different too...I see a post here but I do not understand all....Please write a little bit more why this occures??
thanks in advance.