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SOLIDWORKS DWG SHEET FORMAT & SETTING OPTIONS


Sheet Formats, Sheets and Views: Sheet formats specify the appearance of the drawing sheet, including sheet size, title block, and more. Ownership of items in drawings is dependent on what is active when the item is created. Sketch entities, notes, and other items can belong to the drawing sheet, to an individual view, or to the drawing sheet format. In general, you must activate the owner of an item in order to edit the item. Dimensions and annotations that are attached to model geometry are exceptions to this rule. They belong to the view where they are attached, regardless of whether the view is active when you create the item.


DESIGN A COMPANY DRAWING SHEET & SAVING SHEET FORMAT


Figure 1

To Create a Drawing Sheet for a Part: For me, the easiest way to do this is to...

  1. Creating a simple 3D model. —» File —» New —» in Template —» select Part —» OK —» create a simple model (Figure 1) —»
  2. Entering part's values & properties. —» File —» Properties —» in Property Name —» select Name you want to shown in drawing's Title Block —» select Type —» enter Value/Text Expression —» OK —» see (Figure 2) —»
  3. Drawing sheet size & format setup can be designed per employer's standard or modifying SW's drawing template. Resuming from last step —» File —» select Make Drawing from Part —» select Templates —» select Drawing —» OK —» in Sheet Format/Size —» select a sheet size —» OK to create —» (right side) in View Pallete —» select an Isometric —» drag it onto the drawing —» (left side) close dialog box —»
  4. Attaching simple part to SW's drawing template. Assuming from last step —» RBC —» select Edit Sheet Format —» this is where Sheet Format & Title Block can be modified per company standard —»
  5. Naming & Linking Part's properties to drawing sheet template —» Resuming from last step —» Annotation —» select Note —» place it in drawing's Title Block —» Figure 2 on the left side of screen in A Note dialog box —» select Link to Property —» in Link to property —» check Model found here —» in Property Name —» select the Part's property (create as many name and assign properties to them in this step) —» OK (to close the Link to property diaolg box —» on drawing RMC —» select Edit Sheet —» select Isometric View —» hit Delete key —» Confirm Delete —» Yes —»
  6. Saving Drawing Template. Assuming from last step —» File —» Save As —» select Save as type down arrow —» select Drawing Template (*drwdot) —» in File Name: enter drawing sheet size (ex: A-Vert-Cust) for A size drawing, Vertical format, and Customer drawing —» Save.

Note: Make sure the Isometric View is deleted from drawing before Save or all part properties are linked to drawing. If Isometric View is deleted from drawing before Save, drawing sheet template will displayed SW Document properties only in Edit Sheet Format selection.

Customize drawing sheet formats to match your company’s standard format. Drawing templates contain notes that link to properties. These properties extract information from the part, assembly, or drawing. System properties are automatically available when notes are inserted. Custom properties can be entered on the Summary Information. Custom tab for drawing, part, or assembly documents as appropriate. Avoid overwriting the standard sheet formats that are included with the software.

Figure 2 Design and layout new drawing template and store custom sheet formats in a separate directory.

To link custom drawing sheet template: Start Soliworks —» Tools —» Options —» System Options —» select File Location —» Show folders for (down arrow) —» select Document Template —» select Add —» select the folder where custom drawing template stored —» select Folder —» select OK —» select Yes —» File —» New —» the new tab is created in New Solidwork Documents.

User can link a note to the properties of the model shown in the drawing (the SW-File Name property or user-defined custom property in the model drawing document). If the property value can not be found, the note display Error![variable name]. To show or hide the error message, click View —» Annotation Link Errors.

A linked note can include additional text, and it can include links to more than one property. Ex: to display the current sheet number and the total number of shhets, user can add SHHET $PRP:SW-Current Sheet" of $PRP:"SW-Total Sheets" —» the displayed would be SHEET 1 OF 2 on the first sheet of a two-sheet drawing.

To Create a Drawing Sheet for an Assembly: The same process but insert a simple assembly instead of a part.


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