Yes make the center of the part the origin and mirror half of it.

Also where possible (either this sketch or others) use Equal relations for fillet radii, holes and even lengths of lines that you know will be equal. This will keep you from adding a dimension to each entity. Keep in mind design intent, though - some you may later want to change.

Adding extra relations and making the center the origin definitely reduced the dimensions. Thank you!

Another thing I do is to drive most if not all of a part from one sketch, that way you don't end up with a ton of sketches with dimensions on each sketch. As Master Jack said use equal relations as much as possible. I have found that mirroring is a great way to save dimensions also but beware as if you delete anything that is mirrored it will break your model or cause errors that can be hard to find on complex models.

This is how I would have done this sketch. I hope this helps.

@PProcario, Do you remember the types of relations you used? Did you draw it as one sketch?

I will put a step by step together tonight to show you exactly how I did it. Its all one sketch and very simple to do.

Sorry I have not gotten a chance to put the tutorial together, I have been very busy over the last 3 days. I should get some time tonight to do it.

No worries, whenever you get a chance!

Ok step 1 create the large circle in the middle and dimension it. Make sure to add relation coincident to the center. Then add the center line through the middle of the circle and add a mid point relation to the line and origin, and a coincident to each end and the circle.

Step 2 Create the smaller circle off to the left and dimension it and set the center of the circle with a horizontal relation to the origin. Now dimension from the center of the circle to the origin.

Step 3 Draw a line from the top side of the small circle to the top side of the larger circle and add tangent relations from the line to each circle. It is important that the line is tangent with both circles. Also add a coincident relation from each end of the line to each circle. Now draw the bottom line the same way and add its relations.

Step 4 using the trim tool remove all the bits that are no longer needed like in the picture. The sketch may enter an over defined state which can be fixed by deleting the coincident relation on the bottom of the center line in the big circle.

Step 5 select everything but the center line and click the mirror entities tool, and check copy then mirror across the center line and click ok.

Step 6 If all went well you should have a fully defined sketch with just 3 dimensions. Cheers

Thats great Phil, very detailed! What I was missing most was adding the proper relations to the right parts of the sketch. I also never created the centerline. Thank you for your help!

Glad I could help. One thing I would like to add is be very careful of your design intent. I didn't do it in this example but I never use the origin for setting up relations to parts of my models. This has caused me a ton of troubles when I first started, an alternative is to create two center lines one horizontal and one vertical with a reference point related to the cross section of each line. Then drive all your dimensions and relations off that point. Now if you want that point at the origin set a relation to that point and the origin as being coincident. The reason for this is you can move your part where ever you need it without breaking your relations or your model. This is especially useful on parts used in assemblies. I hope you understand what I mean.