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 the 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 Flow simulations also require 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 Idiot-Simple. (Equal stress on both words). That, in fact, is the problem. It is so simple, that when you use it, you’ve surrendered control over model rebuilds, wetted contact areas, overlapping of volumes, and you get a one-size-fits-all solution that does not, in fact, 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.
Not too terribly long ago, engineering work was fairly compartmented, and the workflow (esp. through larger corporations), went vertically down thru trades: Designer, Engineer, Analyst, Production Engineering, Quality Control, Manufacturing, etc. Computers, Wikipedia, and software like SOLIDWORKS has allowed compression of that workflow, and 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 don’t 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 course…), then you can see why they would try to write a dumbed-down tool to cap the open ends of a model, & 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 way too smart to be using the Lid tool. I want to show you better ways. 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.
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, so might as well make it thick enough that you can easily see the difference, and not accidentally select a wrong face.
Some advantages of this approach:
A1: It is associative to the model – any parametric change will re-build the plug
A2: No additional files to name, vault, and manage
The Main Disadvantage:
D3: We’ve just added to the mass and volume of the housing. If you are doing a flow-only study, (that is, 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 3 of the Solidworks Essentials training can find the Convert Entities icon, so the extra 3 clicks required, (compared to the Lid command), buys you a boatload more robustness.
Multi-Bodies At The Part level
In day one of the 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 advantage only benefits 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 method 1, that I’d like to present:
D4: 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. Not that this is a terrible problem. The study will run, & the results will be correct. But if you like to do hand-calculations to verify your sim results – (good for you!), 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).
Since Method 1 above, does not have this issue, I should have listed it as “A4”. I guess I’ll have to append a summary table of all the good and the bad, at the end of this article.
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. My goal is not to teach it here. 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 1 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 2 other positions. At the same time, I’ll illustrate how to overcome limitation D4, 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.
The variation is this: Once you’ve started sketching on the outlet face, do not create a Convert Entities copy of the outter diameter of the nipple. Instead, I’m showing below, that the plug will be extruded from a Convert-Copy of the Inner Diameter. Of course, 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 of which face is the ‘wetted’ face, easier).
Then, in the next image, I’ve created a linear Pattern of the plug to the 2nd and 3rd 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 3 instances of the plug, one of them built locally, “Top-Down”, and the other two are used as if ‘bottom-up’ copies… and 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 approach to methods 1 and 2;
A1: It is associative to the model – any parametric change will re-build the plug
D2: Requires additional file(s).
A3: Can be assigned Ideal Insulator material properties
A4: The ‘wetted’ face of the plug measured in the CAD is the true flow cross-sectional area.
Now I’m going to cross the wires, by combining ideas from method 2 and 3. Just to prove that, as far as CAD techniques for plugging internal flow is concerned. It’s all good.
Multi-Body Top-Down Plugs In The Assembly
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 3 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.
But 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, in fact. 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.
Now, it is time to throw a curve-ball into this discussion – literally. 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. Consider the next screen-shot, where 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 that 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 – eight pages! 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.
- 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.
- 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.
- 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.
- 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?
- 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.
OK, time to keep score. For the Lid tool:
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
A3: Can be assigned Ideal Insulator material properties.
D4: A measurement of the face of the plug is not the ‘wetted’ cross-section.
D5: 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 1-off study; that I’ll never come back to and edit, ever; and I am not going to be turning on Conduction in Solids. Not terribly often. And when I DO use it, I immediately FIX all the parts in place, to prevent accidental drift. But you might decide to never use it – and you would not be missing anything. It was conceived to close a skill-gap, that YOU very likely do not have, and so you can pick and choose between one of the 4 methods presented above.