Overlooked But Useful SOLIDWORKS Tools: Intersect
SOLIDWORKS is an extremely powerful 3D modeling software. It’s used by a wide range of engineers and designers who all have different goals and use different tools. However, even for the most experienced power user, there’s bound to be many SOLIDWORKS features that aren’t often used.
The Intersect tool is one of these features that too often goes overlooked. This article will act as a short tutorial on how and when to use this powerful tool.
Intersect tool icon, found in the features toolbar.
But first, a quick disclaimer. The Intersect tool requires prior knowledge of how to manage multibody parts in SOLIDWORKS. So, if you aren’t familiar with these tools, consider learning about multi-body parts before diving into this tutorial.
What Is the Intersect Tool?
I learned about the Intersect Tool in the same way I learned about many other useful SOLIDWORKS tools: by struggling. We’ve all been there, trying to bend the software to our will, but just not being able to create what we envisioned. In this case, I was trying to create a part like this one:
The desired geometry.
This is a simple part. However, that post in the center was giving me a headache. I couldn’t use the “Up to Surface” End Condition in the Boss Extrude command because there were multiple surfaces that the extrusion needed to terminate on.
The “Up to Surface” End Condition was no help.
My boss had been watching me struggle. After watching for a few minutes, he finally took pity on me and jumped in to help. He pointed out a magical tool that would easily let me accomplish what I was trying to do.
He told me about the Intersect Tool, which allows the user to create solid bodies from the intersecting regions of two or more existing solid bodies. Users can then delete or keep these resulting bodies depending on the desired geometry.
How to Use the Intersect Tool
Let’s look at that part I was working on. Instead of trying to get the extrusion to terminate at the complicated face, we’ll just extrude it well past the whole outside ring (shown in red). You don’t need to worry about the extruded distance as long as it completely clears the outer edge of the red part.
Pro tip: Be sure to uncheck the Merge Results box in the Boss Extrude property manager.
Two solid bodies, instead of the desired one.
So now, we are left with a multibody part, consisting of our original red solid body and the new, overly long body (shown in blue below) we just created that interferes with the red body.
Two solid bodies, instead of the desired one.
Now what? Enter the Intersect Tool. Let’s activate the tool, found either on the Features toolbar or in Tools > Features > Intersect Tool. Once opened, we see this screen:
Intersect tool Feature Manager.
Now, let’s select our two separate solid bodies and leave the “Create Both” option button selected.
Select the bodies to intersect.
After hitting the Intersect button, we see that the selected bodies have turned yellow. If we hover our mouse over the part, we see that the entire part is now separated into regions. These regions are essentially wherever our two selected parts do and do not interfere with each other. There is also a list of these regions under the Regions to Exclude tab in the property manager.
This is where the Intersect tool really comes into play. When I was first shown this tool, my boss described it to me as a 3D version of the Power Trim sketch tool. One of the best things about the Intersect tool is that it allows the designer to be a little sloppy, if you’ll pardon the term.
Earlier in the tutorial, I said that the distance we extruded the center post did not matter. This is because, as long as it extends past the first part, we can trim away the excess material beyond this point. We just click on the unwanted regions in the graphics area, and they disappear.
Trim away the unwanted regions.
You can also see in the above image that Region 2 and Region 6 are checked in the “Regions to Exclude” box. Once we exit the Intersect tool, those regions will be gone. In the Options tab, make sure the “Merge result” box is checked, or all these regions will output as separate bodies. Once that is checked, let’s hit the green arrow and finish up with the Intersect Tool.
We can see that we now have the exact part we originally wanted and that the blue body has been consumed by the red one. There is one clean resulting body, named Intersect2.
A beautiful part with a beautiful new name.
A word of caution: don’t overuse the Intersect tool. I suggest judicious use. While powerful, this tool can make your design somewhat unstable, especially if it is in a stage where it still might be subject to redesigns.
Remember how the two original bodies were combined into a new one, effectively erasing the original two? This means a few things. One, if you are working with a part that has multiple bodies, you will have to keep close track of the bodies after intersecting them, especially since the tool will rename them. Two, any features created after using the tool will be dependent on that feature in the tree. This means that you won’t be able to move a feature in the tree from after the intersect feature to before it. Three, if you make any changes to features before the intersect feature in the design tree, it will often break the intersect feature.
It can easily be fixed, though.
A simple change in a previous feature breaks the part and gives us the dreaded yellow triangle.
Having said all that, this is still a powerful tool, which in the right circumstances can be extremely useful for complex designs. I’ve only outlined one use for the Intersect tool, but there are many other ways to use it, such as with mold and cavity making, or with surfacing. I encourage you to experiment with the Intersect tool and find out what works best for you.