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Change Drawing file part association?

14 REPLIES 14
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Message 1 of 15
dvandoren
6162 Views, 14 Replies

Change Drawing file part association?

I sometimes create parts that are very similar to one another. (ie. - complex plate, but one part uses threaded holes, while an identical one has through holes, with all holes in the same location). So before now I would have built one part, made my drawing file. Then Copy/paste the part file into the same assembly folder, edit the hole feature of the newly copied part, then have to create an entirely new drawing file for the new copied part.

Is there a way to just copy my already created part drawing, and then just change the part file it used? They are basically the same part, but one uses threaded holes, the other uses through holes. My current way seems redundant and time wasting.


David
14 REPLIES 14
Message 2 of 15
a18cey
in reply to: dvandoren

If you are using Vault the easiest way to do this is "copy design" it does it all for you along with name and file changes. If you are not using Vault look into it.

or do a file save copy as of your initial IDW file and call it another name or drawing number and place an X at the end of the ipt file used to create the first IDW. Open up the second IDW (Created with file save copy as) and you will be prompted to choose the part that goes with it as the reference has been lost due to you placing an X at the end of the original. Simply chose the new ipt and all references and dims will be the same, if you have any custom iprops in the border you will have to redo these manually. Finally do not forget to remove the X from the initial ipt file.


Hope This Helps Edited by: a18cey on Dec 1, 2009 4:46 PM
Message 3 of 15
dvandoren
in reply to: dvandoren

@a18cey - Hey thanks, it works. This seems like a "bass-ackward" way of doing it. I'm surprised A-Desk doesnt have this feature in there. Sometimes I can do dozens of iterations of parts, all with small design changes and with how I like to keep each iteration of parts as their own file, it can take me hours/days to rebuild all the drawing files.


Thanks!

David
Message 4 of 15
Dan
Participant
in reply to: dvandoren

this has been addressed in 2010 bonus pack - replace drawing references tool. you simply save copy as on your original IDW, open the saved copy and swap out the model for the new one using the replace drawing ref tool.

You need to be a subscription user to get it though.
Message 5 of 15
Anonymous
in reply to: dvandoren

Or, you can use the design assistant which is designed for this very thing.
In windows explorer right click on the idw you want to copy and select
"Design Assistant". When that comes up go to the manage tab and copy or
rename as needed. You can also change the file locations if needed and
replace parts in assemblies only. Take a look at it and see if this will
work. It's easier that the rename hassle. Oh just as a reminder when you
open design assistant it will use the current project file you are working
with for file links and locations.


wrote in message
news:6297326@discussion.autodesk.com...
this has been addressed in 2010 bonus pack - replace drawing references
tool. you simply save copy as on your original IDW, open the saved copy and
swap out the model for the new one using the replace drawing ref tool.

You need to be a subscription user to get it though.
Message 6 of 15
Anonymous
in reply to: dvandoren

Hi David,
I would create an iPart and then produce as many drawings out of it as
needed. The way it works you create first drawing of the part, finish it off
and save. Then open that very drawing, save it as another file. In view
editing dialog box select the model you want to be shown in this file (Model
State tab, iParts Member). Done.
But if iParts is not your cup of tea - then you have to do what other
posters have suggested.
Regards,
Igor.

--
Web: www.meqc.com.au
www.boatworks.meqc.com.au
wrote in message news:6297290@discussion.autodesk.com...
I sometimes create parts that are very similar to one another. (ie. -
complex plate, but one part uses threaded holes, while an identical one has
through holes, with all holes in the same location). So before now I would
have built one part, made my drawing file. Then Copy/paste the part file
into the same assembly folder, edit the hole feature of the newly copied
part, then have to create an entirely new drawing file for the new copied
part.

Is there a way to just copy my already created part drawing, and then just
change the part file it used? They are basically the same part, but one
uses threaded holes, the other uses through holes. My current way seems
redundant and time wasting.


David
Message 7 of 15
Bill.Schmid
in reply to: dvandoren

It's just not very clear to me how this works. I went to the "manage" tab and under the actions for the drawing and assembly I selected "copy". Then it changes the entry in the modified column to "requires edit." What's that mean? Help doesn't mention it.

Does anyone know where you can find complete step-by-step instructions for this?

I like my way better.
1. Save Drawing A as Drawing B.
2. Save Asm A as Asm B. (Note: Drawing B will still be looking for Asm A.)
3. Temporarily move Asm A to another directory, I used my Desktop.
4. Open Drawing B. It will be looking for Asm A, but won't be able to find it. So it will prompt for the file to use.
5. Select Asm B.
6. Modify Asm B and the changes will show up on Drawing B. Drawing A will be unaffected.

Bill

> {quote:title=Guest wrote:}{quote}
> Or, you can use the design assistant which is designed for this very thing.
> In windows explorer right click on the idw you want to copy and select
> "Design Assistant". When that comes up go to the manage tab and copy or
> rename as needed. You can also change the file locations if needed and
> replace parts in assemblies only. Take a look at it and see if this will
> work. It's easier that the rename hassle. Oh just as a reminder when you
> open design assistant it will use the current project file you are working
> with for file links and locations.
Message 8 of 15
dvandoren
in reply to: dvandoren

Yeah this just doesnt seem right. For a system that has been designed for optimization and ease of use i'd expect one of two things to be said about this:

A) There is a simple way of doing this....here it is
or
B) You are not following drafting procedure. You should be doing this instead, so it may follow revision, part number or serialization standards.

I have a hard time believing that ADesk made is so in order to start Rev 2.0 you'd have to rebuild parts/drawings/assemblies by hand, over and over again.
Message 9 of 15
Anonymous
in reply to: dvandoren


    When the requires edit appears
you then need to right click on any field that you would like to edit and select
the option you want.  If you right click on the file name and select
"change name" it will bring up a dialog box where you can type in a new
name.  You then hit enter or the open button to have the changes reflected
in the manage area.  Do all changes you want to all files and
locations, then simply hit save and your done.  I woudl really try it out
and play with it a bit.  The software is not that intuitive, but it works
well when you get used to it.


style="PADDING-RIGHT: 0px; PADDING-LEFT: 5px; MARGIN-LEFT: 5px; BORDER-LEFT: #000000 2px solid; MARGIN-RIGHT: 0px">
It's
just not very clear to me how this works. I went to the "manage" tab and under
the actions for the drawing and assembly I selected "copy". Then it changes
the entry in the modified column to "requires edit." What's that mean? Help
doesn't mention it.

Does anyone know where you can find complete
step-by-step instructions for this?

I like my way better.
1. Save
Drawing A as Drawing B.
2. Save Asm A as Asm B. (Note: Drawing B will still
be looking for Asm A.)
3. Temporarily move Asm A to another directory, I
used my Desktop.
4. Open Drawing B. It will be looking for Asm A, but won't
be able to find it. So it will prompt for the file to use.
5. Select Asm
B.
6. Modify Asm B and the changes will show up on Drawing B. Drawing A
will be unaffected.

Bill

> {quote:title=Guest
wrote:}{quote}
> Or, you can use the design assistant which is designed
for this very thing.
> In windows explorer right click on the idw you
want to copy and select
> "Design Assistant". When that comes up go to
the manage tab and copy or
> rename as needed. You can also change the
file locations if needed and
> replace parts in assemblies only. Take a
look at it and see if this will
> work. It's easier that the rename
hassle. Oh just as a reminder when you
> open design assistant it will
use the current project file you are working
> with for file links and
locations.
Message 10 of 15
Bill.Schmid
in reply to: dvandoren

Thanks! That clears it up a bit. Design Assistant does seem very powerful. I'm surprised it doesn't get more exposure. The "where used" function is very useful, too.

Bill

> {quote:title=Guest wrote:}{quote}

>

>

>

>

> {font:Arial}{size:2} When the requires edit appears

> you then need to right click on any field that you would like to edit and select

> the option you want. If you right click on the file name and select

> "change name" it will bring up a dialog box where you can type in a new

> name. You then hit enter or the open button to have the changes reflected

> in the manage area. Do all changes you want to all files and

> locations, then simply hit save and your done. I woudl really try it out

> and play with it a bit. The software is not that intuitive, but it works

> well when you get used to it.{size}{font}
>
Edited by: billschmid5536 on Jan 14, 2010 3:37 PM
Message 11 of 15
Anonymous
in reply to: dvandoren


    One other thing in case you
haven't figured it out yet.  The window at the bottom is for finding all
linked files.  You will see some icons at the top of the lower
window.  Select the ones that relate to the associated files you want to
find.  In the top window select as many files as you want to and the hit
the find files button.  It will go though and find any files of the type
you checked off that relate to any of the highlighted files from the
top window.  Works great when you nedd to copy a whole design and all
related IDW's.  All of this functionality is also built into Vault as well
and in vault it's not as hard to decipher.


style="PADDING-RIGHT: 0px; PADDING-LEFT: 5px; MARGIN-LEFT: 5px; BORDER-LEFT: #000000 2px solid; MARGIN-RIGHT: 0px">
Thanks!
That clears it up a bit. Design Assistant does seem very powerful. I'm
surprised it doesn't get more exposure. The "where used" function is very
useful, too. Bill > {quote:title=Guest wrote:}{quote}
>
>
>
>
> {font:Arial}{size:2} When the requires edit appears
> you
then need to right click on any field that you would like to edit and select

> the option you want. If you right click on the file name and select

> "change name" it will bring up a dialog box where you can type in a
new
> name. You then hit enter or the open button to have the changes
reflected
> in the manage area. Do all changes you want to all files
and
> locations, then simply hit save and your done. I woudl really try
it out
> and play with it a bit. The software is not that intuitive,
but it works
> well when you get used to it.{size}{font} >
Edited by: billschmid5536 on Jan 14, 2010 3:37
PM
Message 12 of 15
dwing
in reply to: Anonymous

I have a question.  I have a drawing of a machined casting (a part).  There are many views and sections.  Now we need to turn that part into an assembly that has some plugs in it.

 

Is there a way to have the drawing point to the new assembly so that all the views can be saved??  The only thing changing would be the addtion of the plugs.  I sure don't want to have to re-draw.  It's a two-sheet E size.

 

I have tried using Manage, Replace Reference Model (only allows part filles),  Design Assistant and Vault but don't know how to get it to work.

 

Dan

 

www.yf.com

www.tactair.com

Message 13 of 15
ltnieh
in reply to: a18cey

Hello Sir,

 

I do not understand your instruction very clearly. 

 

I can save a copy of a model file under a new name.

 

I can save a copy of a drawing file under a new name.

 

But the new drawing file still reference its view contents to the original model file.

 

How to switch the reference view to the new model named part file?

 

When you say put an x behind the name of the part file, where exactly are the sequence of your process?

 

Thank you for your help.

 

Luther Nieh

ltnieh@gmail.com

11/25/17

 

Message 14 of 15
johnsonshiue
in reply to: ltnieh

Hi! The command is called "Replace Model Reference" in Manage tab in the drawing environment.

Many thanks!

 



Johnson Shiue (johnson.shiue@autodesk.com)
Software Test Engineer
Message 15 of 15
ltnieh
in reply to: johnsonshiue

Hello Johnson,

 

Thank you for your help.  It worked very nicely.

 

This is definitely a more direct way to accomplish the drawing and model cloning operation.

 

Thanks and regards,

 

Luther Nieh

11/25/17

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