Proper procedure for creating parts in an assembly?

[pkelecy]

This is pretty basic, but what is the recommended procedure for creating the parts in an assembly?

From what I can see, it looks like there are two approaches:

1. Create a "base" part, drag that into a new assembly, and then use the "Create Part In-Place" command to create the others.

2. Create each part separately (where each is designed and sized so it will fit properly with mating parts) and then dragging each into the assembly, fitting them as I go.

With (1) I can use existing parts to create (include) profiles for use in creating mating parts, which will better ensure that parts fits properly. With (2) I have to know what the mating parts look like (in both shape and dimension) so I can create a part that will fit. But I can reuse this part in other assemblies, if wanted. An "in-place" part appears to be specific to the assembly in which it was created.

Any suggestions? Thanks for the help. -Pat

 

[ryandias]

Whats the difference?

Why do you need to set this in stone?

I am not sure if this is the "prefered" method, but I will draw a part (create) if it is a very strictly defined part, and then create the assembly around it.

Otherwise, when i work with Concept models, I start with an assembly and "create in place" everything.

What benifit would setting the process in stone be?

 

[beachcomber]

I think you may be a little confused about some of the meanings here.
Create-in-Place does not mean that the part is tied to an assembly - it just allows you to see and reference the surrounding parts, but this can be done for any part in the assembly whether created in-place or seperately.
If you do include geometry from other parts you will usually have to open the assembly to edit the part ie. you have to open the "in context" assembly.
Even then the parts can still be used in other assemblies
However, included geometry does not have to be associative. In fact I usually ensure that it isn't, so as to avoid the "in-context" bit and because too many inter-part links can get very confusing - especially when you come to create copies of assembly structures with rev manager.
As ryandias says, you use whatever method is appropriate.

bc.
2.4GHz Core2 Quad, 4GB RAM,
Quadro FX4600.

 

[PatCouture]

The two procedures are related to different type of design workflow. As ryandias mentionned you don't have to stick with one or the other, you can easily combined the two. I tend to use the create-in-place command strickly for custom parts that will be use only for the parent assembly. On the other end for parts that I want to re-use over and over in several assemblies (by that I mean that I copy the part and create a new one with a slight difference, such as a tube with a different lenght) I prefer to stay away from this and then I use peer variables to stay associative.

It's also a matter of designing from top to bottom or from bottom up. With a top to bottom workflow I will make extensive use of create-in-place, inter-part copy and copy sketch. While for a bottom up design I will tend to use part copy combined with peer variables.

I'm worried that I may as well get you more confused. But my point is they are both good method depending on your needs.

A simple advice would be to use as much templates as possible for repeating parts, such as square tube, flat bar, etc.

But still what's good for me may not be as good for you!

Cheers

Patrick

 

[KENAT]

I use a bit of both, and as beach suggests usually drop interpart links once I'm finished iterating.

KENAT,

Have you reminded yourself of faq731-376 recently, or taken a look at posting policies:

http://eng-tips.com/market.cfm?

 

[pkelecy]

Thanks for all the responses!

ryan - I wasn't trying to set anything in stone. Just trying to determine if there was a right approach to doing this, which I now understand depends on the situation (as you indicated).

bc - Yes, I was confused. I was under the impression an in-place part was actually stored in the assembly file. I thought that because I had created one, but couldn't find a separate file for it. I now realize that's because it had been saved to a different folder! Duh! So I'm now starting to understand how this all works.

I do have one other question. Is it possible to create a part based on the profile another part, without the in-place part command (i.e. without being in an assembly). Just curious.

Thanks again for the help.

Pat

 

[KENAT]

You can do an insert part copy but I don't think that's what you mean.

You can also create feature libraries, but again may not be quite what you mean.

KENAT,

Have you reminded yourself of faq731-376 recently, or taken a look at posting policies:

http://eng-tips.com/market.cfm?

 

[beachcomber]

Hi Pat,
Just to expand a little on Kenat's reply
If you are not in an assembly you can do insert part copy.
You can make the resulting feature construction and use this to include edges etc for your new solid, or have it as a solid "base feature" and then build on that.
You can copy/paste features and sketches from one part to another, or copy profile elements from one to another.

If you are in an assembly you can do Copy Sketch from one part to another and have them associatively linked or not.
You can also use Insert Part Copy to copy faces from one part to another (you will need to Edit the part in place to do this).


bc.
2.4GHz Core2 Quad, 4GB RAM,
Quadro FX4600.

 

[pkelecy]

Thanks for the suggestions.

I was basically wondering what other options there were for referencing geometry (ie face profiles) from other parts when creating a new part. So the suggestions were helpful.

I tried the part copy command to see how it works. Looks very useful. I have one question though. I assume I use the "design body" option if I want to use the inserted part as a base feature, and "construction body" if I only want to reference it (in constructing profiles, etc.). Is that right?

Pat

 

[beachcomber]

Hi Pat,
Yes, you are correct in you assumption.
You will also see the options for scaling, mirroring and linking to the original. You can also move it by creating a co-ordinate system in the new part, and the 0,0,0 of the original will be positioned at this system.
You can also import assemblies using Part Copy, although they can sometimes have problems with edge-to-face connections.

bc.
2.4GHz Core2 Quad, 4GB RAM,
Quadro FX4600.

 

[PatCouture]

The part copy command is really a blessing for mirrored parts.

 

[pkelecy]

So are you saying it's better to use part copy to mirror a part, rather than use the mirror command?

 

[beachcomber]

Pat,
Which mirror command do you mean?

If you use Mirror Body in a part file it will create a mirrored copy of your part up to that point - but it's still one part (even if the 2 bits are not joined).
To create an 'opposite hand' part, the Insert Part Copy command is the quickest way, and would normally be the one to use.

There is also a Mirror command in assembly that you should look at in the future, as this lets you create mirrored sub-assemblies.
You can define which components should be mirrored and which are rotated (eg screws). It then creates the Insert Part Copies and builds a new sub-assembly with the parts positioned correctly (but not constrained)

bc.
2.4GHz Core2 Quad, 4GB RAM,
Quadro FX4600.

 

[PatCouture]

For me a practical example that I see a lot is the two sides of a conveyor with holes in them for all kinds of guides, leg and so on. Usually I design the right hand side in sheet metal and then to create the left hand side I go into a new sheet metal file and insert the right hand as a part copy with the design body option checked and also the mirror option while selecting which reference plane to use for the mirror. This way I can get the exact flat pattern of my left hand side if I need it, and it will stay associative with the right hand side.

I hope it helps.

Patrick

 

[beachcomber]

Sounds good to me Patrick.
Exactly the way I would do it.
How does this work in SEwSt - is it still the same, and what happens if you then modify the new part?
Say you move a hole in the copy by 10mm, then go back to the original part and move the same hole by the same amount.
Does the hole in the part copy move another 10mm or does it stay where it is ?
In traditional SE you can achieve the same effect with the direct editing tools and it would move again. ie the new position is relative to the original.

bc.
2.4GHz Core2 Quad, 4GB RAM,
Quadro FX4600.

 

[donyoung]

BC,

that can't be tested at the mo just because IPC is not supported by the current release (ST-Mode). It will come (hopefully) with ST2. Also not implemented is SplitPart, FOA, FOP and SheetMetal as a whole (ST-mode)

dy