Turning off Edit Sheet Format

When I insert a part into a drawing, it switches to Edit Sheet Format, so
that i can not drag the views I want. Does anyone know how to disable Edit
Sheet Format when i insert a part into a drawing?

 

I checked, template is not saved in format mode.

 

There is a system>drawings option for dynamic drawing view activation make
sure it is on.

Corey

 

Now it's now switching to edit format sheet when i insert a part (which is
good) but i still can't drag my views. And i have smooth dynamic drawing
motion and show contents while dragging checked off in my template. What's
wrong here???

 

I was going to ask - how do you know you are in the sheet format? Does the
drawing view disappear? If not, then you are still in the sheet.

WT

 

Lock view? where do i check that? as for the sheet view, i know coz the
drawing disappears and i can edit the boarder text, but that problem is
fixed now, so i just need to figure out how to make my views draggable.

 

I didn't read it right the first time. There may be some mixing of terms
going on here.
In a drawing you have a sheet format that is the picture behind the drawing
namely the title block and border, This "Picture" is refered to as the
sheet format. When editing the sheet format you can edit the title block
but you shouldn't see any views just the Sheet Format. When you exit Sheet
Format you can draw ontop of the sheet format "Picture". This is drawing on
the Sheet when it is in focus. When you have drawing views added ontop of
the sheet the drawing views take Focus dynamicly depending on where the
pointer is. You can lock the focus of each drawing view and draw
specifically in that view. The reason you have all these options it so that
you can keep text where you want it. Text placed on the sheet when it has
focus will not move when a view is moved. Text placed on a view will move
with that view. And In my opinion you shouldn't really edit the sheet
format except when editing the template, because this information can be
lost if you decide to change the standard of your company title block. Most
of the information that is in a title block can be controlled with the use
of custom properties and the information will be residual when you swap one
sheet format for another. IMHO

Clear as mud?

Corey

 

Something not yet mentioned - what version of SW are you on? 2005, 2004,
etc?

WT

 

Thnx, i know all that already. don't worry. The company templates are all
backed up. I edit the templates to my own preferences. My problem right now
is: i have all the boxes checked in system options, so that when i insert
the front view of a part onto the "picture" sheet format, i can simply drag
my mouse to the right to drop in the right view of the part, but it is not
doing this. Right now i have to insert each view of the part individually
and the views do not have parent/child relations.

Sorry if i wasn't clear earlier, i don't know all the terms.

 

Hahaha, one of the most important details....

i'm using 2005

 

Hahaha, that worked! thank alot. you made my day. i've been trying to fix
this for 2days now.

 

Ok, here's what I tried with SW2005 SP0.1.

1. Open a part file.
2. Go to File/Make Drawing from Part
3. Pick the standard SW drawing template.
4. LMB click a location - it defaults to the front view.
5. Move the mouse to the right - click to place that one.
6. Move the mouse to the ortho position and click that one there.

Seems to work every time. This procedure is just to make sure we are all
talking the same thing.

WT

 

First off to insert a projected view you need to use the projected view
tool. This should give you the parent child relationships you want.

Does your template have any predefined views.

When you use the model view command you have the option at the bottom

Start command when
creating new
drawings.

If this isn't checked it won't do it.

Corey

 

Interesting - I don't think I ever noticed that one. It appears in the
registry as:
"Auto-start Projected View command after inserting Model View" under the
General area of SolidWorks. I also could not find any indication of it in
the Tools/Options area which means the only visibility to it is when
starting a new drawing. If, per chance, you turn it off there, the option
doesn't reappear until starting a new drawing.

SW2004 appears to be the same.

WT