in context parts in an assembly

To put it simply, if you have an assembly open and are in Edit Part mode, if you create a relationship to a different part in the assembly, you have now created an in-context piece.

Any of the normal sketch relations - coincident, concentric, convert edges (my favorite), etc. that are used with a piece of geometry in another part creates an external relationship (another name for in- context).

Another method is when you create Extrudes, Cut-Extrudes, etc. where you use Up to Surface, Vertex, Offset from Surface etc. where the surface is from another part in the assembly creates an external reference.

The main issue you need to be aware of is that these external relationships can only be updated in-context of the assembly where they were created. You HAVE TO HAVE the assembly open if you want to see these relationships work properly. These parts should also not be used in more than 1 assembly - which lends itself great towards one- off parts.

There's a good rule of thumb list on Matt Lombard's web site:

Good luck,

Steve O

site:

A guy at work told me that I could make an "in context" relationship between a bolt and a hole in an assembly. Then I could populate an assembly dwg with that bolt into every hole of that size in the assembly. A very big time saver (dont have to mate each bolt to each hole). Is this the same thing you are saying? If I mate a bolt to a hole in an assembly, i.e. an in-context mate, then if bring another bolt into the assembly, it will automatically locate itself in each of the same type of hole? Do I have that correct. THANKS MUCH FOR THE HELP!

First, a simple mate does not create an in-context relationship. These occur at the part Sketch and Feature level, not assembly mate level.

You're looking for a Feature Driven Pattern in the assembly. Use one part with a series of holes either using the Hole Wizard or a linear/ circular pattern and then place your fastener set in the first hole. then you can use the Feature Driven Pattern in the assembly to populate the rest of the holes. No extra mates are created. This is one of my favorite assembly tools.

Steve O

Also take a look in SolidWorks Help for "Smart Fasteners" and "Smart Fasteners Hardware Stacks"

John Layne

Doooh - Forgot all about that. Smart Fasteners should do a good job for hardware.

Steve O

Something that you need to be careful of is if an element in a sketch is "attached" or "linked" to the assembly or just initially referenced. As an example. If a hole location is referenced from Part A onto Part B and if the part A is moved later in the assembly the hole in part B will move accordingly- sometimes causing real problems. Sometimes this can be helpful but for the most part this can turn out to be a disaster.

One approach is to remove the reference constraint in the sketch. The edge or center then needs to be dimensioned or anchored etc. Another approach is to be sure that the "No External Reference" is toggled on. When No External Reference is on, no reference will be created and the hole will not move when Part A is moved in the assembly. This is usually handy because once the hole is located in part B, part A can then be constrained to the hole, just as the real fastener would constrain the two parts together.

Hope this helps,

EdT

EdT,

where is the "No External Reference" located?

Turning OFF External References IS NOT A SMART MOVE. Once you figure out how to utilize external references will save you time 99% of the time. Why in the world do you use a parametric based modeler if you don't use the power of it. You might as well be using a program like Cadkey or Autocad. True, external relations may cause problems in the beginning with circular references but once you understand them, it is a HUGE time saver. If I move a tapped hole or thru hole that has a mating hole, why have to make the same sketch edit in all the parts that this hole affects. Changing one dimension to update 3 or 4 other parts is worth the "disaster" that could happen if you miss one of those holes that was supposed to move. This is almost as helpfull as the good old autocrap days of manually editing a dimension rather than moving the geometry to where it is supposed to be and then giving that file to the CNC programmer to use for machining.

Given the nature of the origional question, External References can really cause problems with someone that is new.

Autocad is not really a 3D program and Cadkey is obsolete, Keycreator is probably not a good investment. Many would say that SW is the best

If you are working on projects that are similar to previous project, then parametrics can be useful. But, for the very first design and there is no idea about what the parts are going to look like, how many parts are going to needed, or how they will relate to each other then I have always found references for this stage of a desing to be very unhelpful. As far as the issue of managing holes that align this is why SW developed Smart Fasteners. I find that it is best to put in most of the fasteners when most of the design looks pretty good. Also, some of the folks that went to SW World have described a new tool in SW2008 that goes through the model to check if all the holes are aligned properly between parts.... it will be interesting to see this tool when it arrives.

billyb, I hope that you find this explanation helpful.

Edt