Hi Guys Please let me know if this question isnt clear. First off I would like to explain how we model and assemble our parts soyou may understand the question more clearly.
We start off by creating a model which we call our "master file" where we do the whole design, after that we create all the parts from a part copy of the "master file" by cutting out the un neccecary body or adding etc.
So when we make the main assembly we would first bring in the "Master file" and then constrain all our parts on top of the "master file" to prevent mistakes and to make revisions easier.
Okay so my question is as follows, is their an easier way to assemble the parts...
You can use the uccorence properties and change the origin to "0" to move the part in the correct position but then it is still not grounded by constaints.
Is their a quicker way to insert a part and then the part will be in the correct position?
Thanks a mill guys.
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Not sure what you are after but I think you want the parts brought in to assembly relative to their position that the were created at in the master file. To do this, hold down the CTRL key when dragging in the parts from the Parts Library tab. This will drop them in their relative position they were created in and ground them at the same time.
I think, it is exactly what nanan mentioned
The only I'm not absolutely confirming is, that it should be one master-multi-body-part
I think there could be several for different areas of the assembly where connections and "interpart" relations can be defined.
A big issue IMHO is, that there is the basic question itself:
"Should there be a interpart relation anyway?"
Or might it be better to use synchronous modifications instead to change things easier and faster without having the handicaps of interpart relations.
As always in live the mix of all these technologies and functions will turn out as the best practicable soluiton, isn't it?
You can model within a part file creating multiple bodies.
This IMHO is somehow similar then other CAD software is/has done, and for me - without knowing NX to much - NX does similar. For me all those products look like this which having everything stored in one single file.
So You have more then one boody (within an assembly I would then use the naming part) can be created.
And they can have relations to each other.
Which are - in that case - simple surface to surface or skecth to sketch relations, as we have done it in parts for a long time.
Those relations give YOu the capapbility to change one "body" (part) with automatic modifying others.
And this without having the need for an interpart relation, since You are only working within one part.
Finally, to let those seperat "part-bodies" having diefferent materials, numbers, properties You can export or expose them to seperate files with an automatic opportunity to send them into an assembly too.
Yeah, the OP is talking about Master Model method. I used this a lot in a previous life. Take an automobile. You wouldn't model the door as a part and the fender as a different part, you'd model the entire body as a single "master model", and then split it up into its constituent parts. Then you use an assembly to bring those parts back together, using the shared origin as the reference point.
It is usually used for complex shapes where the shape flows together between the parts. You use the Part Copy command to insert the master model into a child model, and cut away what you don't need.
You can use multibody parts to get there, but that's a different discussion. Plus, multibody is not meant to replace assemblies. You can get into a fair bit of trouble for doing that.
And Ken definitely nailed it with the method to reassemble.
"Master Model" is just a technique, it's not a named tool in Solid Edge. You can use a lot of tools to achieve the technique. A multibody model can be a master model, and then separate it out to individual parts (publish?).
Master model is a method you use to get parametric/associative chidren of the master, so when the master is changed, the children update.