Using existing drawing for another part 1

[dogarila]

I have 5 parts in an assembly. Each part has it's own drawing. I also have 5 other parts identical with the first 5 in a different assembly. I would like to use the 5 existing drawings to create the drawings for the last 5 parts (they must have their own drawing). What are the steps I should take?

Andrew

 

[MadMango]

I think a simple Save As in the models and drawings of the 5 existing parts to the new models and drawings should do the trick.

Then close everything, and open the 5 new drawings and set their references to the 5 new models that were Save As. "Happy the Hare at morning for she is ignorant to the Hunter's waking thoughts."

 

[dogarila]

Mad Mango,

How do I set the reference of a drawing to another part (already existing)?

These are the steps I would like to do:

1. Create a part P1
2. Create a part P2 as a copy of P1
3. Create a drawing D1 of part P1
4. Using D1 create a drawing D2 of part P2

Is it possible?

Andrew

 

[APPENG]

Andy,

Just exaclty what are you trying to accomplish here?

First, why two copies of the same part?
Second why reuse the same drawing for the other part?

Are you trying to reuse the drawing because you dont want to have to recreate the views?

the reason i ask this, is because my answer depends upon what you want to accomplish

but for what its worth:
yes you can save a part as a copy under a new name.
yes you change the refernced model inside a drawing to point to the copied model...
and yes you can save the drawing as a copy under a new name as well....

you can do this all in one move...

FILE/SAVEAS

click "REFERENCES"

you will see a white area containing two columns called "new pathname" and "current pathname"

select the model that you want to copy in the white area by placing a checkmark in the box adjacent to it.

click again on the name of the part in the new pathname column and type in a new name for it. (be sure to leave the .sldprt extension on it)

click browse if you want to put it in a new directory and navigate to that directory...leave it alone if it's in the same directory.

Click "okay"

type a new name for the drawing in the saveas dialog box,

click okay

but please tell me more about about WHY, I may have some better alternatives for you

regards
Jon

 

[MortenDK]

How about just making more sheets "add sheet"
and then give the header another title?
you can hide features like edges in the dwg sheet, so if the cause is to have identical parts with only difference from each other is a hole or a chamfer, these features are drawn to the part, but excluded individually on the say, drawing sheet1.
The features can still appear on the same part imported to same drawing sheet 2 or 3.
Printing the drawing then gives mores sheets, changes to part size etc. gives change in both parts. Morten K. Thillemann

 

[APPENG]

Well that's why I am asking exactly why he wants to do what he asks, I have a feeling that configurations, mutiple sheets, and other tools may benefit him more than what he is doing now... I'm digging into his business a little in hopes I can find out wht the ultaimate goal is.

jon

 

[dogarila]

Jon,

Suppose we have to design an assembly line with 5 stations. We will call the job A1000 and the stations will be 100, 200, ..., 500. The main layout of station 1 will be
A1000-100-000. Then we call subassemblies in a station using the middle digit of the station number like
A1000-110-000
A1000-120-000
and so on for station 1
A1000-210-000
A1000-220-000
and so on for station 2
and so on to station 5

Details of these subassemblies are A1000-110-001, -002 ...

Suppose we have 2 subassemblies quite similar on two different stations, with many identical details. For example A1000-220-000 and A1000-420-000 share 9 identical parts, A1000-220-001 to A1000-220-009 are identical to A1000-420-001 to A1000-220-009.

Now, I design station 2 which includes A1000-220-000 with its 15 parts (9 similar with A1000-420-000). When I get to station 4 for subassembly 420 I copy 220 using SW Explorer then modify de parts that are no common with 220.

When I create the drawings I will create one for each part called A1000-220-001.sldrw....

When I get to create the drawing for 420 I would like to use the drawings already created for 220 and not redo them from the scratch.

We inherited this system from AutoCAD where it was faily easy to generate similar drawings by changing the information in the title block.

Looks like SW requires a different way of thinking. I would like to be able creat one part with one drawing used in several subassemblies through out a job, or even shared within more than one job. How should I number them? Lets say part P1AAA (sensor bracket) is used 2 times in A1000-220-000, 4 times in A1000-340-000 and 2 times in A1000-420-000. These subassemblies are released at different dates. How do I make sure that in the end I will get 6 parts from manufacturing and not 2 or 4?

Regards,
Andrew

 

[APPENG]

I know what your after, and unfortunately I have to go to work in a minute, I will write you "a book" a little later!

Basically what you want to look at in the mean time is assembly configurations, parametric annotations driven by custom properties, and things of that nature. More about that later,

regrads,

jon

 

[dogarila]

Ok, thank you

A

 

[SnowCrash]

I would think the starting point is to create an assembly of the final resulting assembly, then work backwards, suppressing parts as you go to create configurations of each assembly station or step.
Create a drawing of the final assembled device, then work it backwards also, changing the selected configuration for each view and doing a SAVE AS.. for each configuration drawing.

Crashj 'backwards it at looking am I' Johnson

 

[krishnamurthy]

I suggest you a round about method. Rename the solid part (.sldprt or .sldasm) or assembly.(Hint add TEMP letters to filename). Open the drawing (.slddrw). Solidworks will give you a message telling that it could not find the reference file. Now you browse and pick your new part/assembly. Solidworks will give a message telling that ID is different. Ignore and continue. Save the file under a new name using FILE & SAVEAS command. Be sure to close the .slddrw without SAVING. Rename the initial part/assembly original names. Now you have .slddrw for both old as well as new drawings. Open the new drawing, do the cleaning.

 

[dogarila]

Jon,

I find myself using quite often the method you outlined in your first posting. I'm going to give you star for that.
Thank you,

Andrew

 

[tluxon]

You can also make a new link using the "open" dialog. This works great when you already have a second part file without an associated drawing.

1) Open D1 and "Save As Copy" D2.
2) Close D1
3) Choose Open (as if you were going to directly open D2).
4) Browse to the D2 that is your "Save As" copy of D1 and highlight it.
5) Select the References... button.
6) Under "New pathname", edit the name of the referenced model (P1) to the name of the model that didn't yet have an associated drawing (P2).
7) Select OK, then Open.

Good luck,

Tim

 

[BBJT]

SolidWorks needs to make this task easier!!! Let them know with a enhancement request.

Any way for what it is worth this is how we tackle revisions, like parts etc.

1.)Save or copy part#1 and drawing #1 as part#2 and drawing #2.
2.)Open drawing #2
3.)Right-click in a view and open part #1.
4.)In part #1 pick Reload from the File pulldown then select Replace and select part#2.
5.)Return to your drawing #2 and it will be pointing at part #2.

The reason why I suggested this way to our users is because it is simular to how we rename a part in a assembly.
BBJT CSWP

 

[SnowCrash]

BBJT,
This is an excellent way to handle the problem. Be careful if the overall assembly is open, however, since changes may propagate which are unexpected.
The only tecnique I would add is there should be a template part and template drawing created. This will simplify the creation of the first drawings. I usually create these for each customer or project. I set properties in a different way for several of these since customers want to see different things in the BOM tables.

Crashj 'seen the world from both sides now' Johnson