6/07/2001 Tip#12

= convert entitys

= intersection curve

 

Do you need it?  When did this tool come along into SolidWorks?  Where do I get that tool?  What is it?  In this tip I will discuss all of these and let you know of a very powerful tool that has been introduced to SolidWorks.

First things first, DO I NEED IT?

My answer to you is yes.  If you have ever cut something in half just to get some section properties from a part this will get you the same information but it will be in a parametric sketch.  If you have ever needed to make a projected curve on a face for a sweep or any reason.  This tool will not replace the projected curve but it comes in handy a lot.  If you need to make a helix on a cylindrical face that has draft on it, and you need the exact diameter .010 inches offset from the end of the hole.  All of these are examples of and not only limited to, but where the intersection curve could and does get used.

When did this tool come along into SolidWorks?

The tool was introduced in SolidWorks 2000.

Where do I get this tool?

The tool can be found in two different places.  The first place is View > Toolbars > Customize > Commands TAB > Sketch Tools you can see the tool there just drag it onto the toolbar with the lines and circles on it.  The second place is Insert > Sketch Tools > Intersection Curve.  You can also make a hot key to use this tool if you find that you are using t a lot.

What  is it?
It's a tool that is somewhat like convert entities , with a twist.  Lets say you are working on a simple box.  On the box you make a plane in the middle, your "intent" is to have a sketch on that plane to be exact to the walls of the box where the plane passes through as seen below.

click picture to see larger

 

But lets raise the stakes a little. "What IF" the sides and the top are not the same as they usually are not.  What happens if you convert entities now.  Look what you get.  Not what you want, is it?

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Now that we see what we don't want, what do we use to get our "intent".  I keep saying "intent", what am I talking about.  Well our "intent"  Is to have a ring swept around the middle of this part or where ever the plane passes through the part.  Lets see how to do it.  We choose the plane we need information from and start a sketch (this is for a 2D sketch).  Choose the intersection curve tool .  With a sketch and the intersection tool chosen you can now choose faces that you need information from and they well "convert" to the sketch you are working on but exactly through that plane not as in the example before as it was only the end cap.  The result is below.

       
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Final outcome after sweep no projected curves just selection of the faces I needed to sweep around

 

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That above is using it as a 2D sketch but it can also be used as a 3D sketch.  Let me show you and example of this:

Lets say we are making the famous widget.

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We need to make this "widget a little nicer so how can we do this.  We can use a surface to define the information that we need for our sweep cut for a nice look to our part.

click picture to see larger

 

 

Next to make our intersection curve and a 3D sketch at the same time we just choose the intersection curve tool and start choosing all information that is needed for sweep. (i.e. surface and faces that intersect).  After all information has been selected you can right click on the surface in the feature manager tree and Hide Surface Body.  Below is the 3D Sketch created.

 

click picture to see larger

After cut sweep (Insert > Cut > Sweep) you will get below.

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The sketch entities in both the 2d and 3D sketches can be trimmed extended added for anything you need it for.  Its just another tool to get you model done.

 

SolidWorks Help says:

Intersection Curve opens a sketch and creates a sketched curve at the following kinds of intersections:

• A plane and a surface or a model face
• Two surfaces
• A surface and a model face
• A plane and the entire part
• A surface and the entire part

You can use the resulting sketched intersection curve in the same way that you use any sketched curve, including the following tasks:

• Measure thickness at various cross sections of a part. (See steps below.)
• Create sweep paths that represent the intersection of a plane and the part.
• Make sections out of imported solids to create parametric parts.

To use the sketched curve to extrude a feature, the sketch that opens must be a 2D sketch. Other tasks can be performed using a 3D sketch.

• To open a 2D sketch, select the plane first then click Intersection Curve.
• To open a 3D sketch, click Intersection Curve first then select the plane.