Scaling

[ddlangley]

Why it is when I bring in a part into a new drawing and change the scale. It scales the text on my border, and throws it off.

 

[SBaugh]

In your part or assembly, make sure you have your tools\options\Documnet properties\Annotatons Display\Always Display Text at the same size.

If you don't have it checked, then there is a text scale option above. When you scale your drawing views and since the text is on a scale factor of it's own. Then probably the text is changing to fit the new scale. That is why I always use the option of "Always Display text at the same size".

I hope that helps, Scott Baugh, CSWP
credence69@REMOVEhotmail.com

http://www.3dmca.com

http://home.insightbb.com/~scott.baugh/

 

[ddlangley]

I tried that and I wasn't able to select that option in the drawing properites. Plus whenever I scale the part that I bring into the drawing it scales the border too. I don't understand why it does this. If I use the default template from SW2001 it will not scale the border. So I used the default template to create a new company border bringing in a dxf. and saved it as a template. When I use the new template that I created it scales the border.

 

[meintsi]

When you say the default templates work correctly it gave my an idea.
Are you creating your templates correctly?

Open a blank template, right click on the backgroud, and edit sheet format.

Now add your custom changes, and change back to edit sheet the same way before saving as a new template.

I think this might make your border scaling problems disappear.


Remember...
"If you don't use your head, your going to have to use your feet."

 

[ddlangley]

In SW2001 I'm not able to import a dxf into a blank template. When I try to open a dxf in 2001 and make it a drawing template in doesn't seem to work properly. I go to edit sheet format and my dxf disappears. Once I save as a drawing template and then try to use that template. It still scales the border when I bring in a part or an assembly.

 

[SBaugh]

If you "Edit Sheet Format" the lines in the drawing should be blue. If you have the option of picking "Edit Sheet format" then the lines should be grayed out. If this isn't the case then you have saved your default template the wrong way. You will need to go in and edit that template and save it with the option "Edit Sheet Format" in the menu.

This can be confusing! God knows I still have to mess with it from time to time, when I haven't done drawings in awhile.

If none of the above works you may want to consider reinstalling SW.

Best Regards....and Good Luck, Scott Baugh, CSWP
credence69@REMOVEhotmail.com

http://www.3dmca.com

http://home.insightbb.com/~scott.baugh/

 

[meintsi]

Here's what you need to do...

For bitmaps, tiffs, jpegs, etc...
Setup your new template this way:

Go to edit sheet format before the
INSERT>OBJECT>CREATE FROM FILE>(browse to location) command.

But when trying this, I agree with your statement that .dxf's do not import correctly into a blank template. But I found this work around for you:

1)Import your dxf normally into a blank drawing.
2)Highlight the dxf on the drawing and use the CUT icon on the toolbar.
3)Right click in the background and choose "Edit sheet format".
4)Use the PASTE icon now.
5)rememder to go back to "Edit Sheet" before saving as your new template.


Make all your changes while working under the "edit sheet format" command. Go back to edit sheet (border will turn grey), and save as template.

Any changes done under "edit sheet format" should never scale when you scale the properties of the sheet. If it this does, follow Scott's suggestion of reinstalling SolidWorks.

Good Luck....


Remember...
"If you don't use your head, your going to have to use your feet."

 

[ddlangley]

the cut and paste worked well. Thank you very much for all your help. There for a while, I was becoming very furstrated at this program. Again, thanks a bunch!