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To save a template
Save as type: Drawing Templates .drwdot
save to the same directory as your current templates and when starting a new file it will be in the templates list.
You can also save the Sheet Format separately if you want
File>Save sheet format
This controls the sheet size and the title block
this in normally changed by right clicking on the drawing sheet and selecting Properties
the only way quick way I know of to change units, arrow sizes, text of an existing drawing is to use a macro. I am sure you can find more extensive examples if you look at some of the SolidWorks Bloggers sites that have lots of macros posted but here is a quick example of a VBA .swp macro
Dim swApp As SldWorks.SldWorks
Dim Part As SldWorks.ModelDoc2
Set swApp = Application.SldWorks
Set Part = swApp.ActiveDoc
Part.SetUserPreferenceIntegerValue swUnitSystem, swUnitSystem_Custom 'CUSTOM UNITS SYSTEM
Part.SetUnits swFEETINCHES, swFRACTION, 16, 0, True 'FEET-INCHES 1/16 4 DIGITS ROUND
Part.SetUserPreferenceDoubleValue swDetailingDimFontHeight, 0.0254 / 8 '1/8"
Part.SetUserPreferenceIntegerValue swUnitsMassPropMass, swUnitsMassPropMass_Pounds 'SETS MASS PROPERTIES TO POUNDS
Part.SetUserPreferenceIntegerValue swUnitsMassPropDecimalPlaces, 2 'SETS MASS PROPERTIES TO 2 DECIMAL PLACES
Part.SetUserPreferenceIntegerValue swDetailingDimensionStandard, swDetailingStandardANSI 'ANSI STANDARD
Part.SetUserPreferenceIntegerValue swDetailingDimFractionStyle, swDetailingDimFractionStyle_Stack 'STACKED FRACTIONS
Part.SetUserPreferenceIntegerValue swDetailingDimFractionScaleIndex, swDetailingDimFractionScale_100Percent 'FRACTION SIZE
Part.SetUserPreferenceToggle swGridDisplay, False 'GRID OFF
Part.SetUserPreferenceToggle swDetailingDisplayAlternateSection, True 'ALTERNATE SECTION VIEW
Part.SetUserPreferenceDoubleValue swDetailingDimBentLeaderLength, 0.003175 'DIM BENT LEADER LENGTH 2.54/100/8
Part.SetUserPreferenceToggle swUnitsLinearFeetAndInchesFormat, True 'TURNS ON 2'-4"
Part.SetUserPreferenceDoubleValue swDetailingArrowHeight, 0.0015875 'ARROW HEIGHT 2.54/100/16
Part.SetUserPreferenceDoubleValue swDetailingArrowLength, 0.0047625 'ARROW LENGTH (2.54/100/16) * 3
Part.SetUserPreferenceDoubleValue swDetailingArrowWidth, 0.003175 'ARROW WIDTH 2.54/100/8
As Garrett suggested, you can create the template for the new drawings. For copying to old drawings try this Excel macro "copydocoption" by Stefan Berlitz. This excel sheet is designed to copy SolidWorks document option from one document to another.
Thanks guys, this is great! if you ever need help with renderings let me know!
What I would like to know is, how do I get Solidworks to simply SAVE THE SETTINGS I ASK FOR?
You have to do PROGRAMMING and run SCRIPTS to get your preferences set in Solidworks?
I've saved templates, I've saved templates within templates, and I STILL get freakin' Century Gothic.
Sorry about the caps. But somewhere in a chain of hundreds of checkboxes, there's a checkbox I didn't check. Or a template within a template within a template I didn't save. Or something.
Take a deep breath.... :-)
Where are your templates saved to and are your Tools > Options > System Options > File Locations > Document Templates pointing to where you saved your templates?
After that go to Tools > Options > System Options > Default Templates and check the radio button to Prompt user to select document template. Also browse the Part, Assemblies and Drawings on that same screen and set the locations you have your templates saved to and what you want to be selected as default. The radio button will give you the option to change from the default.
Sorry, Anna. By Friday afternoon I was "fit to be tied."
Our VAR reps are coming in tomorrow--poor fellows.
Thanks to all, i had exactly the same problems as Patrick, all resolved now
There's two types of settings. System and Document. System settings are the same for any document you open. Document settings are controlled by the document itself.
That's a nice pic Anna