[eduhmaia]

Hi!

I'm using FlowSight, which is the Ensight that comes with FLOW-3D v11.

I'm trying to analyse sediment scour data from a .flsgrf file, but not in the entire block; say I want to ignore the 10% closer to each wall (for example, in a 20 cm x 30 cm x 300 cm sand box, only the inner 16 cm x 24 cm x 240 cm matters to me because of wall effects).

How can I do that? More specifically, I want to plot the mass (or volume) of sediment over time. Information for the entire block is available as history data without the need to query, so can I "trim" the history data to the region I want or do I need to calculate the sediment part volume?

Thanks in advance

[Marina G]

Hi,

If you want to examine only a region of the fluid domain, you can create an inside box clip and do your analysis only on this part. Select the fluid domain -> Create -> Clip. Set as Tool: Box. A box will appear in the viewport. Place it so that inside it there's the region you want to analyze (you can drag/move it interactively on the viewport, or in the Clip edit widget, toggle on Advanced, you can change its parameters). Then, set as Domain: Inside and create the clip. This will create a new part that is the elements of the fluid domain inside the box. You can now do your analysis on this new part instead than the original fluid model part.

The query that you have in the query list for the sediment mass vs. time has been loaded from the Flow3d dataset, so it is calculated for the entire dataset and can not be changed in EnSight. You will need to re-calculate this quantity (by using the calculator tool) and re-create a plot of this new quantity vs. time (by using the query/plot ability of EnSight).

Hope this is clear. Let us know if you have more questions.
Best Regards,

Marina Galvagni
CEI Software Support Engineer

[eduhmaia]

Hi Marina, thanks for the prompt response.

I was able to crop the domain using box clip. However, when trying to calculate Vol() function for that new part (called BoxClip in the attached screenshot), the results are always zero.

What am i doing wrong here? I want a plot of the sediment volume contained in the box clip over time.

Once again thanks!

[Marina G]

From the attached image, it looks like the clipped part is only a surface (so, 2D elements). This would give you a Volume = 0, as there are no 3D elements.

You can verify what kind of Elements compose a part by simply selecting the part, going into Query -> Show information -> part. This will tell you what kind of elements are present in the part.

What is probably happening is that you are selecting a part other than the fluid domain when creating the Box clip part. Make sure that the selected part is the fluid that contains the 3D elements (should be part 1?).

Hope this helps.
Bests,

Marina Galvagni
CEI Software Support Engineer

[eduhmaia]

Originally Posted by Marina G

From the attached image, it looks like the clipped part is only a surface (so, 2D elements). This would give you a Volume = 0, as there are no 3D elements.

You can verify what kind of Elements compose a part by simply selecting the part, going into Query -> Show information -> part. This will tell you what kind of elements are present in the part.

What is probably happening is that you are selecting a part other than the fluid domain when creating the Box clip part. Make sure that the selected part is the fluid that contains the 3D elements (should be part 1?).

Hope this helps.
Bests,

Marina Galvagni
CEI Software Support Engineer

Thanks again, Marina.

I don't want information about fluid volume, but sediment volume instead. When FlowSight reads .flsgrf data, does it come as a surface or 3d volume?

Edit: in the posted screenshot, the fluid part is Isosurface - 1 and the scoured sediment part is Component - 1# ~f3d.

[Marina G]

When EnSight reads .flsgrf data, it loads is as volume elements (the Block 1 part). If you want to have the sediment part as a 3D part, you probably want to use an isovolume, not an isosurface. Indeed an isosurface is a part composed only by 2D elements, while an isovolume is all the cells for which the value of the variable is between two values you've set - therefore, it's composed by cells, i.e. it's a volume part, on which you can calculate the Vol().

Hope this helps.
Bests,

Marina

[eduhmaia]

Thanks once again.

How can I generate such isovolume? Can it be read from the .flsgrf somehow or do I need to use volume rendering? Because I've been trying to create volume renders from the sediment parts before and they don't look like what comes from the .flsgrf.

[Marina G]

You probably have a variable called "Fluid_fraction" or similar, that is 1 where the cell is all fluid, and 0 where it's all non-fluid (sediment).

Select the Block part -> right click -> Edit -> Isosurfaces. Set as the "variable" this variable. Change the type from Isosurface to Isovolume. Place as "min" and "max" two reasonable values - for example, 0 and 0.5. Then, create. This will return a new part that is the collection of all the cells for which the Fluid_fraction is between 0 and 0.5, i.e. your sediments. As it's a collection of cells, it's a 3D part.

Now, calculate Vol() on this part. You have the volume of the sediment.

You mention volume rendering. This is something that changes the representation of the part: you will see the part colored by one of the variables, with transparency as a function of the variable itself. It's useful to create informative images, but doesn't change the geometry of the part - so no, this isn't useful in this scenario.

Let me know if this isn't clear of you have more questions.
Bests,
Marina

[eduhmaia]

Originally Posted by Marina G

You probably have a variable called "Fluid_fraction" or similar, that is 1 where the cell is all fluid, and 0 where it's all non-fluid (sediment).

Select the Block part -> right click -> Edit -> Isosurfaces. Set as the "variable" this variable. Change the type from Isosurface to Isovolume. Place as "min" and "max" two reasonable values - for example, 0 and 0.5. Then, create. This will return a new part that is the collection of all the cells for which the Fluid_fraction is between 0 and 0.5, i.e. your sediments. As it's a collection of cells, it's a 3D part.

Now, calculate Vol() on this part. You have the volume of the sediment.

You mention volume rendering. This is something that changes the representation of the part: you will see the part colored by one of the variables, with transparency as a function of the variable itself. It's useful to create informative images, but doesn't change the geometry of the part - so no, this isn't useful in this scenario.

Let me know if this isn't clear of you have more questions.
Bests,
Marina

Couldn't be any clearer, thanks! I'll try this method.

[eduhmaia]

Glad to say it worked!

So, to all the people that will ever read this thread in the future, here's the sequence I did:

1. Simulate sediment scour at FLOW-3D.
2. Open .flsgrf file on FlowSight. It'll show parts Block 1 and Isosurface-1 by default.
3. Right-click Block 1 on the parts list and go to Isosurface. Select packed_sediment_volume_fracion_Restart on the scalar variables list. It'll create a new part called "Isosurface part".
4. Right click the newly created isosurface. Change its type to Isovolume under "Creation". The constraint I used was High with Max=(my packing fraction defined in Flow-3D). This will finish the isovolume creation.

5. Right-click the isosurface again. Go to Create - Arbitrary Clips and use the Box Tool, with Domain = Inside. My FlowSight is a bit bugged so I can't specify coordinates right away (program resets to displayed coordinates), so I click the "Create with selected parts" at the bottom. It'll create a new part called "Isosurface part +".
6. Right click the clip part and then Edit. Check the Advanced box at the top right corner and then enter Origin and Length for the box. Click "Set tool coords" to see what you are doing.

7. With "Isosurface part +" selected, click the calculator tool button on the toolbar above the viewports. Search for Vol() function and create it.
8. Find Vol under Constants on the Variables panel. Right-click it and then "plot over time". Voilá! The result is posted below, I colored the clipped part but that's optional.

Thanks Marina

[zhouyu3092070]

Thanks all. A very good guide.