You can make the base parts, make an assy, then add the holes and select "Propagate feature to parts". The holes will be exactly lined up.
Thanks for your response. So do I make the outline/base of the part then overlay it with the part I am trying to model and then add the holes in the assembly and select propagate feature to parts? I am not positive how to add holes withing the assembly.
Or you could just use the tool built-in to SWX as Jim describes and provided the link for you to learn how to do it.
Jim Wilkinson has answered the question about comparing the geometry.
If you want to have the holes perfectly aligned there are a couple of ways to accomplish the task. First, if the two parts are almost identical, you can do a Save AS of the existing part and save it as a new number. This will have an identical part that you can modify however you desire. Or you can start an assembly in which the two parts are mated together however you want them, in this case one would be perfectly overlapping the other Then you can make assembly cuts to create new holes in both parts at the same time. In doing this you will want to propagate the feature to the parts as shown below. If there are more than 2 parts in the assembly you can also select which parts to make the cuts in.
You can also make the assembly and then make the part you want to edit active using the icon shown below.
This will allow you to edit that part and make any changes you want to it. If you want to create holes in the active part that are exactly like the holes in the other part, while you are in the sketch mode you can select the convert entities button and then select the edges of any features in the non-active part that you want to place in the active part.
Doing this will allow the features in the new part to follow the copied features in the old part if they are changed as long as you do not break the links.
Have I given you enough to go on yet?
Other wise just ask and someone will help.
That helps a lot. I am essentially trying to recreate existing parts as sheet metal parts so I can assign it a set k-value and bend radius. It has just been taking a long time adding the holes in the exact locating when there are a lot of holes. I will try the convert entities feature and see if it helps.
Yes, you can use the Compare Geometry option in the Compare Utility to compare geometry of two different parts. Here is the help for the Compare Utility:
I hope this helps,