Is there a simple, straightforward way to assembly parts similar wiht a concept similar to the snap points that are found in Visio? The models to be built will only vary in inner mechanics which are all pre assembled, but for the most part be very similar and rather simple in outward appearrance. I'm looking for a very quick way for Solid Edge to understand which relationships should be automatic (aligning certain faces automatically) and certain standard heights (1HU, 2HU, etc) to allow for users who don't necessarily know the program well to quickly add subrack drawers into a server cabinet.
Not really. Easiest would be to use coordinate systems in the Assembly that coorespond to coordinate systems in the parts and subs and use the Match Coordinate Systems relationship but would require some setup. You might try Duplicate Component as it will maintain orientation of the duplicates components based on a source feature and a target feature such as a hole.
Sounds like you are trying to use Solid edge as a sales configurator tool or something along those lines. Solid Edge was not built for that but there are a few add-on apps that can do that for you but again requre setup to make it end user friendly.
I just created a model of drawer packs that is the most complicated model I have created to date.
I use ordered sheet metal. All the parts are assembly driven located and sized using assembly planes.
The main trick I used was one plane for each drawer. A series of offset planes was used. If one of the drawers is not in that design, it's space becomes 0. The holes that drawers slides then collapse on the next drawers holes.
Attached is a screen shot of one piece of sheet metals sketch.
The decision you have to make up front is the maximum number of drawers.
One interesting trick I used for that model was an odd vs even set of logic in the variables. The slides come in 2" increments but the drawers are designed in 1" increments. so I had to offset holes 1" based on the even or oddness of the depth.
Thank you! I also have a question for my 2D drawings. When I dimension them, it gives me no input on the distances, and if I change them it won't change the drawing, only the number and show it isn't to scale. Is there any way to change this so that my drawings will change when I alter dimensions?
If your drawings are comprised of drawing views of the 3D model, you must double click on your drawing view to open the model and change it there. Solid Edge does not allow changing the 3D model from the drawing.
If your drawings are comprised of 2D elements drawn in the draft environment, then make sure when you place dimensions that "Maintain Relationships" is on and the Dimension "lock" option is set.