Blocks !!!

[btcoutermash]

I am running SW2004 Sp3.0. I was wondering if anyone could help with this problem I am having. When I insert a block on a drawing, it become associated to the views. So when I move the views, it moves also. Does any one know how to prevent this from happening without going into sheet edit and placing it at that time?

 

[TheTick]

RMB on sheet--> "Set Sheet Focus" before inserting block.

 

[macduff]

btcoutermash,
When I use blocks I RMB "Edit Sheet Format" and insert them in there. This is usually when I do drawing notes, tables revision blocks etc...not associated with the drawing view. When I done, I switch back into RMB "Edit Sheet"

I hope this helps,

macduff

 

[CorBlimeyLimey]

You could also create an Empty view & place your block in it. You can use Set view focus to ensure the correct view is selected or simply highlight the empty view before inserting the block.

from (the City of) Barrie, Ontario.

Support bacteria - they're the only culture some people have

 

[Standing]

Macduff,
This has nothing to do with your question.
We used to put our notes and revision blocks on the template. At the time it sounded like a good idea. Our company has changed its name twice since starting SolidWorks. We had to change the logo on our drawings. With the notes and revisions on the template caused great trouble. I would suggest you not put anything on the template that could not be changed with replacing template. Who knows your company may get sold and the logo may change.


Bradley

 

[lnrdr]

You can also use the "Lock Sheet Focus" command which allows you to see the view while placing your block. To use this command left click on sheet in the model tree, To unlock the focus do the same.

 

[Standing]

We have a Visual Basic program that places our notes onto the drawing. If we do not hide the views or place the notes before placing views, the notes will move with the movement of the views.

Bradley

 

[macduff]

Bradley,
I didn't refer to templates in my thread response. I use blank templates, and insert my notes as needed (using blocks or text) in "edit sheet format". When I switch back to "edit sheet", I can move my views independently without drawing notes moving with the views.

btcoutermash,
This will work if you do not have a VB program.

Have a good day,

macduff

 

[Standing]

Macduff,
Yes I do understand.
When you do a Reload of your drawing template, do your notes disappear? Just wandering.


Bradley

 

[macduff]

Bradley,
My templates consist of:

assembly
part
B-Size
C-Size
D-Size
E-Size

All these are set to the company standards and network file paths I have set-up for users to point point to them.
I also have set-up users to point to blocks, dimension favorites, BOM templates, Revision tables etc...(you get the point)to standardize drawing practices. My standard drawing notes are set-up in a "dimension favorites" folder which I created.

So.........getting back to your question. When a user creates a new drawing, he or she would grab one of my templates (file, new) which only contains the title block and drawing frame. Then insert there drawing notes by:
1)RMB edit sheet format
2)select the text fuction ("A" Note icon)
3)select the "load favorites" (this path needs to be set
in the tools, options, file path, dimension favorites)
in the "text favorite" panel.
4)select your standard note or notes.
5)place it on your drawing
5)ok
6)RMB edit sheet (this gets you back to the master draw
space as i call it)
7)start creating your drawing views

You could make your views first and notes second, that's not the point I'm making. But it keeps everything standardize. That way if a specification changes, let's say......an inspection note, ASTM 1444. I can go into that folder and change that specific note, and the other users will see the change when I file it. The nice thing about it, it doesn't change automatically across the board on old drawings. That would require an ECO againist the drawing that has been already released.

So...........answering your question. When I reload that drawing, no nothing disappers.

Sorry for be long winded,

macduff

 

[Standing]

macduff,
Sounds like you have a very nice setup. Thanks for the answer.

Bradley

 

[macduff]

Thanks for nice comment Bradley. I spent a lot of hours on setting these features up and then some.

It's funny, my co-workers here are starting to call the software.....Colinworks.

Colin
(aka-macduff)

Have a great 4th of July

 

[Standing]

Colin,
Your Welcome.
It is nice to know that I am not the only one out there.
My co-workers here are calling our tools “Brad CAD Tools”


Bradley