Similar drawings

[KevinPinks7697]

I need to create several parts, complete with detail drawings which are very similar. How do I go about this? First I create the first part and then do the drawing for that part, then I save everything. Next I open the original part and "Save a copy as" save it as a new name, but I am not sure how to update the drawing so that the next part has an updated drawing, rather than create a whole new layout with dimenisons and everything.
Thx
Kev

[Anonymous]

This is very easy with Vault's copy design capability.

With Design Assistant (opened from Explorer or off the Start Menu-IV Program
Group) in Manage Mode, open the finalized part.

Highlight it and in the lower pane, check the IDW icon and hit search.

Up top, copy the IPT, then copy the IDW in the lower pane.

Hit the save button and it will create a new IPT and IDW that are linked to
each other.

QBZ


wrote in message news:5024964@discussion.autodesk.com...
I need to create several parts, complete with detail drawings which are very
similar. How do I go about this? First I create the first part and then do
the drawing for that part, then I save everything. Next I open the original
part and "Save a copy as" save it as a new name, but I am not sure how to
update the drawing so that the next part has an updated drawing, rather than
create a whole new layout with dimenisons and everything.
Thx
Kev

[Anonymous]

Kev:

Assuming your first part is modelled and detailed, open the idw and
'Save Copy As' to the other file names. Now from Windows Explorer use
Design Assistant to open each idw, copy the ipt file name to the new
name. Any changes you make to the new ipt will be reflected in the
matching idw.

Richard




kpinks wrote:

> I need to create several parts, complete with detail drawings which are very similar. How do I go about this? First I create the first part and then do the drawing for that part, then I save everything. Next I open the original part and "Save a copy as" save it as a new name, but I am not sure how to update the drawing so that the next part has an updated drawing, rather than create a whole new layout with dimenisons and everything.
> Thx
> Kev

[Anonymous]

I read your post yesterday on this topic but I'm having trouble following
how you accomplished this task.

I created a part: "Hub part 1" and made a copy of it and renamed it "Hub
part 2" and added an additional hole.

I created an IDW from Hub part 1, did a "save as" and renamed the new IDW
"Hub part 2".

This is where I get lost.

I opened the "Hub part 2" IDW from design assistant and "Hub part 1" from
design assistant and now I'm not following how you copied or from where you
copied the ipt file name from and where your copying it to.

Any help is greatly appreciated.

Thanks,



"Richard Hinterhoeller" wrote in message
news:5025026@discussion.autodesk.com...
Kev:

Assuming your first part is modelled and detailed, open the idw and
'Save Copy As' to the other file names. Now from Windows Explorer use
Design Assistant to open each idw, copy the ipt file name to the new
name. Any changes you make to the new ipt will be reflected in the
matching idw.

Richard




kpinks wrote:

> I need to create several parts, complete with detail drawings which are
very similar. How do I go about this? First I create the first part and then
do the drawing for that part, then I save everything. Next I open the
original part and "Save a copy as" save it as a new name, but I am not sure
how to update the drawing so that the next part has an updated drawing,
rather than create a whole new layout with dimenisons and everything.
> Thx
> Kev

[Anonymous]

Here are the steps for a simple "one-part-one-drawing" situation:

1) Create part "Hub part 1"
2) Create IDW "Hub part 1"
3) Make a copy of IDW "Hub part 1" and call it "Hub part 2"
4) Open IDW "Hub part 2" in Design Assistant
5) Select the "Hub part 1" -> Action --> Copy --> Change filename
6) Hit Save

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"Scott Mason" wrote in message
news:5025422@discussion.autodesk.com...
I read your post yesterday on this topic but I'm having trouble following
how you accomplished this task.

I created a part: "Hub part 1" and made a copy of it and renamed it "Hub
part 2" and added an additional hole.

I created an IDW from Hub part 1, did a "save as" and renamed the new IDW
"Hub part 2".

This is where I get lost.

I opened the "Hub part 2" IDW from design assistant and "Hub part 1" from
design assistant and now I'm not following how you copied or from where you
copied the ipt file name from and where your copying it to.

Any help is greatly appreciated.

Thanks,



"Richard Hinterhoeller" wrote in message
news:5025026@discussion.autodesk.com...
Kev:

Assuming your first part is modelled and detailed, open the idw and
'Save Copy As' to the other file names. Now from Windows Explorer use
Design Assistant to open each idw, copy the ipt file name to the new
name. Any changes you make to the new ipt will be reflected in the
matching idw.

Richard




kpinks wrote:

> I need to create several parts, complete with detail drawings which are
very similar. How do I go about this? First I create the first part and then
do the drawing for that part, then I save everything. Next I open the
original part and "Save a copy as" save it as a new name, but I am not sure
how to update the drawing so that the next part has an updated drawing,
rather than create a whole new layout with dimenisons and everything.
> Thx
> Kev

[Anonymous]

Scott:

Starting with Hub1.ipt and Hub1.idw:
1/ Open Hub1.idw
2/ 'Save Copy As' Hub2.idw. (If you were to open Hub2.idw, it would be
looking at Hub1.ipt)
2/ From Windows Explorer (not from IV), RMB on Hub2.idw and open using
Design Assistant.
3/ Along the left side of DA, you have three options, select 'Manage'
4/ In the row with Hub1.ipt, select the button in the action column.
5/ Select 'Copy'
6/ In the 'Name' column, right click Hub1.ipt and select 'Change Name'
7/ The File Open dialog box will display and you can rename the file to
Hub2.ipt
8/ In the top menu bar select 'Save' to save the changes.
9/ Close DA

You now have the file Hub2.ipt in your folder and it's connected to
Hub2.idw with all the dimensions attached. Now you can modify Hub2.ipt
and the idw will follow.

Richard

Scott Mason wrote:
> I read your post yesterday on this topic but I'm having trouble following
> how you accomplished this task.
>
> I created a part: "Hub part 1" and made a copy of it and renamed it "Hub
> part 2" and added an additional hole.
>
> I created an IDW from Hub part 1, did a "save as" and renamed the new IDW
> "Hub part 2".
>
> This is where I get lost.
>
> I opened the "Hub part 2" IDW from design assistant and "Hub part 1" from
> design assistant and now I'm not following how you copied or from where you
> copied the ipt file name from and where your copying it to.
>
> Any help is greatly appreciated.
>
> Thanks,

[Anonymous]

Richard,

I was creating the "Hub part 2" ipt file when I created the IDW file and
wasn't getting the concept of how the link would be created.
Makes total sense now.
Thanks a bunch, much appreciated.


"Richard Hinterhoeller" wrote in message
news:5025489@discussion.autodesk.com...
Scott:

Starting with Hub1.ipt and Hub1.idw:
1/ Open Hub1.idw
2/ 'Save Copy As' Hub2.idw. (If you were to open Hub2.idw, it would be
looking at Hub1.ipt)
2/ From Windows Explorer (not from IV), RMB on Hub2.idw and open using
Design Assistant.
3/ Along the left side of DA, you have three options, select 'Manage'
4/ In the row with Hub1.ipt, select the button in the action column.
5/ Select 'Copy'
6/ In the 'Name' column, right click Hub1.ipt and select 'Change Name'
7/ The File Open dialog box will display and you can rename the file to
Hub2.ipt
8/ In the top menu bar select 'Save' to save the changes.
9/ Close DA

You now have the file Hub2.ipt in your folder and it's connected to
Hub2.idw with all the dimensions attached. Now you can modify Hub2.ipt
and the idw will follow.

Richard

Scott Mason wrote:
> I read your post yesterday on this topic but I'm having trouble following
> how you accomplished this task.
>
> I created a part: "Hub part 1" and made a copy of it and renamed it "Hub
> part 2" and added an additional hole.
>
> I created an IDW from Hub part 1, did a "save as" and renamed the new IDW
> "Hub part 2".
>
> This is where I get lost.
>
> I opened the "Hub part 2" IDW from design assistant and "Hub part 1" from
> design assistant and now I'm not following how you copied or from where
you
> copied the ipt file name from and where your copying it to.
>
> Any help is greatly appreciated.
>
> Thanks,

[Anonymous]

Here is another solution: After you have created hub2.ipt and hub2.idw from your original hub1.ipt simply rename hub1.ipt to hub3.ipt (in IV). Now when you try to open hub2.idw it will ask you to relink, choose hub2.ipt and save after it is open. Now change the name of hub3.ipt back to it's original name of hub1.ipt. Done!

[KevinPinks7697]

Sorry Quinn, but how do I copy the IPT in the upper pane and copy the IDW in the lower pane? I do not know anything about the Design Assistant.
Thx
Kev

[Anonymous]

Right Click on the "Action" button and select Copy.

Then Right Click (or double click) on the filenmame cell and rename it.

The "changed" lines then turn yellow indicating a change.

Once both files are copied/renamed, hit the save button up top and it will
write out the new linked copies.

After it does this, notice that it will revert back to showing you the
"original" names because the "copies" you made were just created and placed.
This is sometimes a confusing aspect of DA.

To see the new linked files(in DA), you need to open the new file explicitly
(in DA) and do a IDW search.

QBZ


wrote in message news:5025634@discussion.autodesk.com...
Sorry Quinn, but how do I copy the IPT in the upper pane and copy the IDW in
the lower pane? I do not know anything about the Design Assistant.
Thx
Kev

[KevinPinks7697]

This is an assembly, so I open the original assembly in DA, copy ythe assembly (1020-0004.iam), then select IDW and do a search, then rename the IDW in the lower pane. So right now all I have in the lower pane is 1020-0005.idw, there are no (ipt) files in the lower pane. This is where I am stuck

[Anonymous]

The IPT's are in the upper pane under the IAM.

You have to select (turn blue) everything (that you want to work on/copy) in
the top pane in order to get a successful search in the bottom.

You have to do all your renaming/copying all at once BEFORE you hit the save
button.

QBZ


wrote in message news:5025660@discussion.autodesk.com...
This is an assembly, so I open the original assembly in DA, copy ythe
assembly (1020-0004.iam), then select IDW and do a search, then rename the
IDW in the lower pane. So right now all I have in the lower pane is
1020-0005.idw, there are no (ipt) files in the lower pane. This is where I
am stuck