Tutorials and training materials focus a great deal on how to push the buttons with your Flow Simulation software. But the first (and most important) step is your model preparation. That’s mostly done in CAD. A lot of hotline calls that seem to be about failed boundary conditions or bad meshing, really end up being about the model prep.

Sometimes model prep involves stripping away small features or parts to simplify the mesh. But SOLIDWORKS Flow Simulation also requires added features or parts to serve as constraint boundaries, mesh refinements, control volumes or most especially lids, which plug your inlet and outlet areas and allow the CAD system to recognize the flow volume as internal. Lids are important.

The Mission of The Lid Tool

You are not reading this article because you can’t find the Lid tool or you don’t understand how to use it. The Lid tool is simple. In fact, it is almost so simple that when you use it you’ve surrendered control over model rebuilds, wetted contact areas, overlapping of volumes and a one-size-fits-all solution. But on the contrary, this solutions does not even fit most. So if you are a trusting soul, you can skip reading the remainder of this article – and quite simply, don’t use it.

See. Look. You’re still reading. I knew you would. Somebody out there is going to expect me to defend a statement like that, and I guess YOU are that somebody. OK, let’s start with a little background.

Background of the Lid tool:

Not too terribly long ago, engineering work was fairly compartmented, and the workflow (especially through larger corporations) went vertically down through trades: Designer, Engineer, Analyst, Production Engineering, Quality Control and Manufacturing. However, over time computers, Wikipedia and other software like SOLIDWORKS have allowed compression of that workflow. Nowadays all those trades can even reside within one skull. So please understand, that the Lid tool was written to solve a problem that I probably no longer have.

The Lid tool is old. If we were to assume that CAD models were always assembled by “Draftsmen” and that flow simulations were the province of “Analysts” whose time was much too valuable to be wasted in taking a CAD training courses, then you can see why they would try to write a dumbed-down tool to cap the open ends of a model and quickly prepare it for an internal flow study. No CAD expertise required. But if you’ve taken the four day SOLIDWORKS Essentials training and logged maybe two or three weeks of mouse-time building simple Extrudes and Revolves, then you are already too advanced to be using the Lid tool.

Better Ways to Create Lids

I want to show you even better ways to create lids in SOLIDWORKS Flow Simulation. So the rest of this article will be an overview of at least four ways to plug your models, comparing and contrasting each approach for advantages. In fact, there is no magic to plugging a leak, and there’s practically no wrong way to do it (except, perhaps, to use the Lid tool). We’ll use this simple air manifold below from a fish tank as the base example for all our techniques. We’ll assume that three outlets are in use, and three are plugged.

Approach 1: Simple Features at the Part Level

The simplest approach is often the best. Across the 1” inlet opening, we’ve added a solid extrusion that re-uses the outer diameter via Convert Entities of the housing. The thickness of the extrusion does not really matter. But when you select a face of the plug to apply an inlet Boundary Condition, you must click on the inner, wetted face. This might as well make it thick enough that you can easily see the difference and not accidentally select a wrong face.

Advantages:

A1: It is associative to the model – any parametric change will re-build the plug

A2: No additional files to name, vault, and manage

Disadvantages:

D1: We’ve just added to the mass and volume of the housing. If you are doing a flow-only study where the “Conduction in Solids” option is off, then this does not matter. But when heat conduction is considered, then the added mass is another pathway for heat to flow which could affect both the steady-state temperature distribution and the time to soak-out the part.

Anyone who has made it to day three of the SOLIDWORKS Essentials training can find the Convert Entities icon, so the extra three clicks required (compared to the Lid command) buys you quiet a bite more robustness.

Approach 2: Multi-Bodies at the Part level

In day one of the SOLIDWORKS Advanced Parts course, you learn how and why to create multiple solid bodies within a single part file. But I find that about half of the students in an Essentials class discover this anyway (mostly by accident), so you end up having to explain it sooner. Thus, with a single additional click, to clear the Merge shown in the Extrude dialog below, you change the plug to a separate solid body. Assuming that your SOLIDWORKS license is up to the current decade, the Flow solver will treat separate bodies in a part, exactly the same way it treats parts in an assembly. Most importantly, you can assign them separate material properties. So by changing your Plug bodies to all be an ideal insulator, you’ve averted the only real weakness in method 1 (D3 above).

The additional advantages only benefit you in a Conduction problem:

A1: It is associative to the model – any parametric change will re-build the plug.

A2: No additional files to name, vault, and manage.

A3: Can be assigned Ideal Insulator material properties.

But there is a subtle disadvantage, compared to approach 1, that I’d like to present:

D1: A measurement of the ‘wetted’ face of the plug, using the CAD tools, will give a larger area than the actual meshed surface area computed by the flow solver.

Because the Plug body does not merge with the housing, it retains a surface area that is dictated by the housing O.D., not the I.D. The study will run, and the results will be correct. But if you like to do hand-calculations to verify your sim results, especially if you are calculating energy balances or reaction forces across inlet/outlet faces – you can’t let yourself be fooled into thinking that the CAD measured surface are of the plug is the actual inlet area. Instead, use the Results – Surface Parameters plot to report the actual wetted face area computed from the mesh.

Approach 3: Plugs as Top-Down Parts in the Assembly

I will refer to this method, taught as part of the Advanced Assembly class, for you more advanced CAD users. Not that this approach is ever required, but I need to cover it en-passant so I can get back to a wrap-up discussion of the Lid command. So, when is an Assembly treatment useful? 

If your study is already an assembly, it might include a number of purchased-parts or at least parts that get referenced in many other situations, not simply in this one simulated assembly. Then you might not want to burden the parts with extra configurations and extra features/bodies; that could be confusing to other users of these files. This is a sensible reason to build all your lids (or control volumes, mesh refinement regions, porous media etc.) as separate parts and include them at the assembly level. It is less effort to hide/show your lids when they are separate parts. You can build one lid top-down, then deploy it as associative instances in many other locations, so there’s only one new file to manage. And often, folks have a lot more experience with assemblies than they do with multi-body parts, so there’s just the old-habits thing.

For my example, I’ll build one plug as a top-down part and then pattern it into two other positions. At the same time, I’ll illustrate how to overcome the limitation mentioned above. In the image below, I’ve already inserted the Manifold part with the inlet face plugged as a body into an assembly – then you can invoke the Insert Part command.

Once you’ve started sketching on the outlet face, do not create a Convert Entities copy of the outer diameter of the nipple. Instead, the plug will be extruded from a Convert-Copy of the inner diameter. To seal the outlet with some finite surface area, the plug must be extruded inward, not outward. Or, as I’m showing below, you can do a Mid-Plane extrude, thus making the plug thicker and the discernment easier.

Then, in the next image, I’ve created a linear Pattern of the plug to the 2^nd and 3^rd port on this side. If the ports were not all in a row, I could have dragged copies of the first plug, and then mated the copies to the other ports. This is still surprising to some folks – that I can have three instances of the plug, one of them built locally “Top-Down” and the other two are used as “bottom-up” copies. This does not confuse SOLIDWORKS at all. 10 years ago or more, this would have been a no-no. Every year, life gets better!

Comparing this to the first and second appraoch, here are advantages:

A1: It is associative to the model – any parametric change will re-build the plug

A2: Can be assigned Ideal Insulator material properties

A3: The ‘wetted’ face of the plug measured in the CAD is the true flow cross-sectional area.

And disadvantages:

D1: Requires additional file(s).

Appraoch 4: Multi-Body Top-Down Plugs In the Assembly

Approach 4 crosses the wires, by combining ideas from appraoch 2 and 3. In the next image, I’ve started a top-down part file on the opposite row of outlets, and I’ve sketched a single rectangle that is big enough to close off all three holes. This is fast, easy and… probably not a good idea.

I wanted this picture to support the following point: Speed and convenience usually costs us something. In this example, I said we were going to simulate two of these nipples as closed and one as open. So I need to put a pressure boundary condition on the middle outlet. Since there is only one CAD face to apply the pressure condition to, it will apply to all three, and I’ve lost that ability.

Let’s take the discussion further; What if all three outlets were open to a common downstream pressure? Then this single plug face would not prevent me from running the study. But it would prevent me from applying three separate Goals to monitor the flow rates, and I would only be able to report the net outflow. I would not be able to measure the flow balance.

I can use the Multi-body approach, to put three separate plug bodies into this one top-down part. Consider the extrude operation below. It is the same part. I have simply deleted the rectangle and replaced it with three uses of the Convert-Entities command, selecting the inner diameter of the outlets. This treatment will work fine for a flow study.

All of these plug techniques are made easy by the fact that the outside faces at every inlet/outlet are planar, and the flow path, perpendicular to that face. Sometimes we don’t have it so easy. Consider the image below where I’ve made one simple change to the manifold. The inlet is on a curve, instead of a straight run.

If you look back at methods one and two, you see that this curved inlet does not change a thing because both of those plugs were built on the outer, planar face. And although it is not a requirement, I used method three to introduce building a plug that seals against the inside face of the inner diameter. That method isn’t going to work very well if the inner diameter is a curving face. In the next screen-shot, the Extrude dialog shows the plug extended some distance into the inlet. On the left, just the preview alone shows that a straight-line extrude will result in a singular, line-to-line contact on the exit face. On the inside radius of the bend, the plug pulls away from the wall. On the outside radius of the bend, the plug violates the wall.

This problem is purely geometric, and as such, there are multiple solutions available in SOLIDWORKS. You could create the plug as a revolve feature. You could make the plug diameter slightly bigger, so it interferes all the way around and then do a Boolean subtraction operation to remove the overlapping volume. But really, how fancy do you really need to get?

It depends upon your flow analysis. If you are not considering thermal effects – specifically, if you have not turned on Conduction in Solids – then it is OK to have overlapping solids in your assembly. So making the plug diameter 5% bigger and doing a straight Extrude would work fine. However, if you DO have solid conduction, then every place where two or more solids overlap is confusing. Which material properties to assign to cells in this area? Sometimes the software cannot guess which properties to apply, and in such cases, the cells become ‘open’ – that is, the default fluid – and your study could leak.

Properties of the LID tool

So, you’ve read this far – NOW do you trust me? We’ve just seen four variations on CAD techniques for plugging inlets and outlets that do not need the Lid tool at all. And we’ve seen how they stack up against each other. But, on the same criteria, how does the Lid tool stack up?

The image below shows the expanded feature tree of my same air manifold after having run the Lid tool and clicking seven faces. Gosh, that was fast and easy. The problem with the Lid tool is not just the things that it does, but also the things you naturally assume it did, but it did NOT do. So I’ll review in detail.

1. The lids are not mated in place. Notice that every LIDx part has a (-) symbol before it in the feature manager, indicating that these parts are free-floating. If you select a face or edge of a LID, but accidentally keep the mouse button down too long, so it ‘looks like’ a drag operation to the CAD, then these parts will joggle, leaks open, and your study fails. So you should at least FIX them all in place, the instant you have created them. But even if you do – If you then make parametric changes to any parts of mates, the lid positions will not update.
2. Notice that the only feature in the LID7 history is “Imported1”. These parts are ‘dumb’ solid bodies with no history. They are made via a macro – a modified Method3, as above, except the extrudes are then saved out to STEP format, then re-imported to scrub them clean of any history. So again, any parametric model changes to the Manifold – the lids will not update, and might need to be re-created.
3. Look closely at the zoomed-up image of the inlet LID, below. Not only is the lid a straight Extrude, it is also over-sized (by maybe 5%) – this was done to guarantee a seal against the side walls, in the event an inlet is curved, as we noted in Method 4. So, for a flow-only study, no thermal effects, this will always work. And, if you have Conduction in solids turned on, this will frequently be a problem.
   
4. Every lid is another new part file, with the same naming convention – LID1, LID2, etc. How are you going to manage your Flow simulations within a PDM environment?
5. For this last point, I show below a copy of the “Coletor” model from the Flow Sim training class – it has 6 outlet faces, and each face is perforated by 1 flow path, and 2 bolt holes. Check out how many LID part files there are in the tree. Clearly, 12 of those files are irrelevant. But the Lid tool proceeds from a geometric survey of the selected faces, not a larger understanding of the model closure, so you have to (or should) delete 2/3 of the LID features that we just conveniently obtained.

Advantages:

A1: Can be assigned Ideal Insulator material properties.

Disadvantages:

D1: It is not associative to the model – any parametric changes could require re-creating them.

D2: Maximum possible number of files to name, vault, and manage

D3: A measurement of the face of the plug is not the ‘wetted’ cross-section.

D4: Can create “Irregular” cells, confusion that defaults to leaks.

Bottom line, despite all I’ve said thus far, I actually DO use the Lid tool, sometimes when I’m in a hurry, for a one-off study that I’ll never come back to edit or if I am not going to be turning on Conduction in Solids. And when I do use it, I immediately fix all the parts in place to prevent accidental drift. It was conceived to close a skill-gap. But with today’s resources, there are many work arounds for it.

Want to learn more tips and tricks? Check out our SOLIDWORKS Flow Simulation training courses.