# rectangular extruded hole centered on rectangular surface?

I just started with SolidWorks student edition, and have gone through the 30-minute tutorial. That was enough to get me started on much of
the stuff I want to do. I'm amazed at how powerful yet easy-to-use it is, and I'm sure I've barely scrached the surface.
One of my parts has a rectangular face, and I wanted a rectangular hole extruded into it, with the center of the hole locked to the center of the face. I was able to do that by putting ceterlines of the face into the sketch, and centerlines of the hole, and then using Add Relation to make both vertical centerlines colinear, then both horizontal centerlines.
What I'm wondering is whether there is some easier/faster way to do that?
Thanks! Eric
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Well, that's exactly what centerlines and relations are supposed to be used for - to add some intelligence and design intent to your model.

Draw a diagonal construction line from corner to corner of your original face. Then draw a similar one to your sketch rectangle. Then you can add a such relation that the midpoints of the diagonal construction lines are coincident. (RMB on the first line -> Select Midpoint, then ctrl-select the another line and add a Midpoint relation).
-h-
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I wrote:

Heikki Leivo wrote:

I understand that. I just meant that maybe there was some shortcut for creating a rectangle centered on another rectangle or something.
Since posting the question, I did notice that selecting two centerlines brings up a property manager in which I can just click "colinear". That's faster than how I was doing it before.

Clever, thanks!
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If the second rectangle is offset from the first by the same amount on all 4 sides, then the quickest method is (probably) to select the face and then use the sketch "offset" command.
It will add the 4 new lines of the rectangle and make them all offset by a predetermined amount from the original edges.
John H
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Most times I will use the diagonal construction line method as described above. However here is another way that involves a Reference Point. This is not a Sketch Point its under the Reference Geometry toolbar.
Insert/Reference Geometry/Point/Center of Face. turn on View/Ponits Insert Sketch of the Hole and use the Point for the center.
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If it makes sense in the larger context of your part design, you might want to center your initial rectangle on your origin in one or both directions. (Use the diagonal line/centerpoint method mentioned by others.) This can help when you add new features that are symmetrical. This will also often help later when you are putting the part into assemblies, as you can mate using your basic planes, making it easier and more robust.
Jerry Steiger Tripod Data Systems "take the garbage out, dear"
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I'd agree that this is by far the best method overall. The only negative being that SWX doesn't include the origin in lightweight parts, so you have to resolve them to constrain to it - how stupid is that!
John H
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John H wrote:

Might constraining the mid-point of the line to two planes work better?
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Jerry Steiger wrote:

You're right. I've started doing that, and it is quite helpful.