Troubleshooting Solid Body Counts and Volume Discrepancies in Your 3D Modeling Workflow

In this video, we're going to review solid body and volume management. For this video, simply follow along. There won't be any new modeling.

Now, let's go ahead and check how many solid bodies we have in our part. We go up to here at solid bodies, we see 99. All right.

Now, if your solid body count is too low, the first likely cause is you have a pattern somewhere with the incorrect number of instances, and you'll need to correct that. So let's start with the feature patterns. The, there we go.

And if you highlight the feature, you can see the information that created it,  and you'll be able to find that number of instances there,  which you can change here in this box if you so desire. That should be five. This feature pattern ought to be six.

Oh, there's that six right there. Okay. Excellent.

Once you've confirmed that those are okay or corrected your mistakes,  you'll want to go through each of the sketch patterns. You can find your sketch patterns by grabbing one of the pattern surfaces. It'll highlight that feature that created it, highlight the sketch in that feature,  and it'll give you all the information that was used to create that sketch,  including the number of instances in the patterns that are being used.

You can double click here and then just change the number if it needs to change. This first one is 21, and the second should be 14. All right.

Now, the second likely scenario is you accidentally merge bodies in the boss extrude command. If that's the case, you'll need to go through each of your boss extrudes,  edit the feature. Oh, let's start with the first one, or sorry, the second one.

You'll need to go through, edit the feature, and uncheck merge result. The last likely scenario is you need to fix the selected contours in one of your extruded boss commands. You may have some solid line sketch entities that need to be central lines or vice versa.

I will show you how that likely happened and how to fix it. For that, I'm going to open up a new part. Oftentimes, as you know, we will start with a center rectangle.

We'll set some dimensions, 20 × 20. And this is just to establish a basic space. If I want to make, say, the legs of a table as we've done before,  I'll go ahead and create those legs and extrude what I've created.

But here's the problem. This outside rectangle still has solid lines. So the program is going to think I want to extrude, say, this space in the middle.

So I'm going to go ahead and make sure these lines are central lines by highlighting them all and clicking for construction. Now we'll only extrude these four. Had I not done that, let's go ahead and bring that back.

When I go to model this feature, it doesn't know which parts to model,  or it may have modeled the wrong ones inadvertently. If we go to selected contours,  we could potentially model this entire middle cross. That's not what we want.

We would actually want to model these four. But again, had this outside rectangle just been made of center lines,  the program would have no problem identifying exactly which contours to model. All right, I'm going to close that out.

Now we have a few instances in our model where we created outside rectangles or other shapes to use as center lines so that we could have references for the pieces that we eventually model. You need to go through and make sure that the things that should be center lines are center lines,  and the things that should be solid lines are solid lines. That likely occurred in either the ground plane sketch or the height sketch.

So I would encourage you to review those videos if you need to. All right, if your solid body count is too high,  the first likely cause is you have a pattern somewhere with the incorrect number of instances,  and I've showed you how to correct that. Second, you likely created new unwanted bodies during an extruded cut command.

As we know, extrude cut can turn one body into multiple bodies if it cuts cleanly through. You'll need to go through each of your extrude cut commands and check the number of bodies before and after that command is executed. We can do that by grabbing this blue bar,  going to the very top cut extrude,  taking account of how many bodies are here, 48,  and how many bodies occur after, 51.

That's because we cut some of these planks into two pieces. If this occurs and it's the wrong number,  or maybe it occurs in another extruded cut command,  you probably cut a piece in half that you didn't mean to do. So you need to make sure that you need to fix your sketch if that is indeed the case.

The good news is we only have to check three extrude cut commands to make sure we got it right. Now, if that doesn't work, the next likely scenario is you created a body by accident by having one too many closed sketch entities in a sketch. If I were to go back to when these beams were first created,  and we made a lot of rectangles in this particular sketch,  but say by accident, we made a teeny tiny rectangle kind of off to the side that we didn't notice.

Our program would have interpreted that as a solid body that needs to be created. You may have done this, but done it in a way where it's hidden somewhere where you can't see it. You want to go through your sketches and make sure that those types of entities don't exist.

Another way to handle that would be to go through each of your solid bodies in this dropdown menu, highlight them,  and just make sure that that is a solid body that you actually want to be in your model. Whereas if I were to say highlight this solid body,  I'd say, oh, wait a minute,  that doesn't look like it belongs. Let's go ahead and fix the feature that created that particular element.

We'll do that by highlighting it,  going to delete, remove it, and now it's gone. All right, it's very important for this course that you maintain the same count of solid bodies that we have moving through each of the lessons. Now let's look at volume.

First, let's make sure you have the evaluate tab added to your command manager. You can do that by going to command manager,  right clicking on any one of the tabs and checking that evaluate is on. In the evaluate tab,  we have a button known as mass properties.

We click it and it tells us a lot of mass properties of the volumes that we have here in our graphics area. One of them is the overall volume in cubic inches. Now ours should match.

Let's go ahead and click out of this. Now looking at the volume,  that's what it should be correctly. In fact, I'll bring that back up again.

If you have the correct number of bodies and you know that each body is meant to be there,  but your volume is still too high or too low,  you likely have sketches where you created shapes that are a bit too large or too small. That probably occurred because again,  SolidWorks likes to prompt references and sketches that you may not want. It's possible that you accidentally grabbed a coincident reference or a colinear reference that SolidWorks gave you.

This would result in an overall volume that is close, but not perfect. The most important factor in this course,  again, is the number of solid bodies. A difference in volume,  especially one that is very small,  say a few cubic inches here or there,  is probably okay.

Although it is an indication that you need to pay more attention as you are building sketches. A volume disparity that is too high,  say anything over 10 cubic inches, however,  must be dealt with as soon as possible. The first likely cause is that you have built your model in millimeters and not inches.

You'll need to fix that and go back through your sketches and fix any smart dimensions that are incorrect. Let's go ahead and close this out. The second likely cause is your global variables are not what they should be.

So let's go ahead and look at those now. We'll go to Tools, down to Equations. Here it goes.

I should bring this menu up. Check to make sure that your global variables match what is shown here. All right.

The third likely cause is that you mistyped a smart dimension somewhere,  most likely in one of your two reference sketches at the top of your feature tree. So let's look at those now. If we highlight ground plane,  we can see all the dimensions that were used to create it.

Many of them are global variables,  but there are a couple that aren't. For instance, this is 90. And that indicates 90 inches.

This is 36. You'll want to make sure that those are correct. In our height sketch,  we set an overall height to the second floor at 72 inches.

You'll want to make sure that that's correct. And anywhere that you have a sketch that features a smart dimension that isn't a global variable,  you'll want to go back and make sure that matches what is shown in the video. All right.

Thank you. In the next video,  we're going to make a complex sketch pattern for the first time,  and we'll use that to prepare the stairs. We will also make the top two stairs.