SOLIDWORKS Tech Tip: Task Scheduled Drawings

[fa icon="calendar"] June 25, 2015 / by TPM Admin

Mike Staples, TPM Application Engineer

If you want to speed up the process of creating SOLIDWORKS drawings, the SOLIDWORKS Task Scheduler is a great tool. Using tasks, you can batch create all of your drawings now or at a specified date/time. You'll still need to open them and make adjustments but it certainly saves time.

Note: SOLIDWORKS Professional or Premium is required.

Just a few steps and you'll have your drawings created:

  1.  If you don't already have one, create a template with predefined views (see further down for more on this)
  2.  Launch the SOLIDWORKS Task Scheduler (Start > All Programs > SOLIDWORKS 20xx > SOLIDWORKS Tools > SOLIDWORKS Task Scheduler) (or just press the windows key and start typing task)
  3.  Choose create drawings
  4.  Browse to your drawing template (with predefined views)
  5.  Click add folder (you can do individual files if you like). Check the box for include subfolders if desired.
  6.  Set the filetype (parts or assemblies) in the File Name or Type Field.
  7.  Set when you want the task to run and where the drawings should be created and click Finish

SOLIDWORKS Tech Tip

You can monitor the progress in the Task Scheduler (click Refresh to update).

SOLIDWORKS Tech Tip

SOLIDWORKS Tech Tip

SOLIDWORKS Tech Tip

Here's a few tips:

  1. Since placing model items is best done after creating all of your detail and section views, I recommend not having model items (dimensions marked for drawing) checked in your drawing template document properties. Instead, import them using model items after you've created all of your views.
  2. Often assembly drawings are different than part drawings so you may want to create separate drawing templates and run one task for your parts and another task for your assemblies.
  3. If your parts/assemblies are in EPDM be sure to check them out before clicking "Finish" in the task scheduler.

 

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Drawing templates with predefined views. Start a new drawing and insert predefined views to populate the views you typically place (usually front, top, right, and iso). You can either create each individually and align or place one and use projected views. For the individually named views place each one and select the orientation in the property manager, then use the alignment from right-click menu in the view. Alternatively, place one (probably front) and use projected views for the rest.

Note: the predefined view command is not on the command manager by default - it's under Insert > Drawing View > Predefined (or use the command search).

Set your document properties to include things like centermarks, centerlines, dimensions marked for drawing, dual dimensions, precision, centered dimensions, parenthesis, etc (see images below).

This will be the starting point for your drawings so pick what will be used most often. When you open the drawings you'll often need to add/remove views.

Once you have things setup just click save as and choose drawing template for the save as type.

SOLIDWORKS Tech Tip

SOLIDWORKS Tech Tip

Topics: Manufacturing, SOLIDWORKS

TPM Admin

Written by TPM Admin

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