Best Practise when creating parts within an assembly.

[Rickpage76]

Hi,

My question is about the creation of parts within an assembly.

When creating multiple parts for use in an assembly, I've been making each part individually using (good practice) to fully constrain the parts to the planes & axis so it's very easy to line things up using the origin planes, I then attach them together within an assembly with the relevant constraints.

This is clearly the wrong way to do it, as should I change a dimension in say the main part I then need to adjust a dozen other files that were affected by this change.

So creating a part within an assembly is where I get confused.

When asked by inventor where should I create the sketch for a new part?

Should I choose the cut edge of an existing part or just select an origin plane.

It seems whatever I choose the part is created in the middle of nowhere.

Many Thanks

Rick

Don't flame me too much I've learnt via youtube 😞

[Rickpage76]

Practice 🙂 Spell Check

[Sergio.D.Suárez · Accepted solution]

Hello, I think there are several ways for what you are looking for
which is to reflect changes in an assembly when modifying a piece within it.

On the one hand in a part you could model and redefine the planes of origin or even the ends with extrude "to" a plane or a face of another part of the assembly to work with an adaptive piece. For this you must have selected these boxes in options of the application.

You could also work with derived parts and link parameters of a piece with another piece of the same assembly, so that by varying a dimension the new dimension of the new part will vary. To do this you must link the parts from the parameter box -> link -> select part and select parameter of part

Another way would be to model a multibody, create a part file, where each solid within represents each part of your assembly (recommended for assembly of not many parts and where the parts are not repetitive) and once the assembly is complete, create new ones components from the solids generated in the file. (It is known as muscle modeling)

Another way similar to the previous one would be to model a piece file, complete only with sketches, as a skeleton of the master assembly, with these sketches parts will be created with the creation operations within each part file. (It is known as skeletal modeling)

In each of these examples if they are well formulated you can change a parameter in one piece and the rest of the dependent pieces will be updated observing the respective changes

[Rickpage76]

Hi, thanks for taking the time to make a detailed reply.

I'll give those methods try.

cheers

[mdavis22569]

Let's ask a different question:

Why are you creating the parts in the assembly?

I would put all the parts on the same plane when ever possible (that's me) 

[Rickpage76]

Hi, I've been thinking about your reply, wondering why you would draw everything on the same plane.

Why would you not think ahead and sketch on the planes best suitable for the part?

As an example if you was drawing a car I'd sketch the bonnet as I looked at it from the front or top, most likely using the xz plane. For the doors I'd chose maybe the xy plane as they are side on.

If you sketch everything on the same plane when it comes to assembling the parts your always rotating stuff about.

I know you can constrain it in the correct places but it just seems to add more work flipping it around ect.

Back on the original topic I've included a quick assembly & would like to know if this is the best way to create the side panel for the box (part being created within the assembly).

The way I've made the side panel works but is this the best way to do it?

Upon opening the side panel file on it's own the planes are all over the place & i couldn't ever use them to align anything in future.

This is what I can't grasp, is it important?

many thanks