sheet format Archives - SolidWorks Legion

Automatic Border tool works its wonders

Check out SOLIDWORKS’s Automatic Border tool and how it makes editing your Sheet Formats so much easier than old fashioned sketching!

SOLIDWORKS has the amazing Automatic Border tool for Sheet Formats. You don’t need to sketch your drawing borders from scratch. You also do not need to edit many sketch objects to update your borders.

The Automatic Border tool allows you to control all elements of your drawing border and associate those with drawing zones which are intrinsic to the drawing sheet. The tool has many functions to provide to you the ability to make and edit your borders to your exact needs.

To support ease of editing your Sheet Formats, a tab is available on the CommandManager called Sheet Format. This tab includes the tools Edit Sheet Format, Title Block Fields and Automatic Border. To find the Automatic Border tool:

Choose Edit Sheet Format to switch to Sheet Format mode. Then, select Automatic Border tool.

On a newer template created in SOLIDWORKS 2016 or later, your border will highlight as orange. (If you have an older Sheet Format or you are trying to incorporate your old Sheet Format from another CAD application, see SOLIDWORKS Help.) In the Automatic Border PropertyManager, select Next to edit your existing border.

The first page of the PropertyManager is for legacy (pre-SOLIDWORKS 2016) Sheet Formats. If you have a newer Sheet Format, just skip this first page by selecting Next.

On page two of the Automatic Border PropertyManager, you have many options to edit your border.

Zone size and Margins

Zone Size groupbox allows you to establish your zone distribution and region.

The 50mm from center option under Distribution allows you to use a common size and placement regardless to sheet size.

Evenly sized option allows you to automatically divide the sheet up into evenly sized zones, including a custom number of rows and columns.

Under Regions, you can set zones to fit within the sheet’s margins (Margins) or the sheet’s extents (Sheet).

Margin groupbox allows you to establish where your border appears on the sheet in terms of distance from the sheet extents. You can set the border’s line font and thickness. Also, there is an option to allows you to include double-line border called Double-line border.

Independent Border groupbox is a less commonly used option that allows you to place your borders separately from margins. This is only useful if you have unusual distribution of sheet zones that do not take the border into account, with the same Right, Left, Top and Bottom settings as Margins.

Zone Formatting

Zone Formatting groupbox provides several highly specific settings to control the display of zones within the border.

You have the option to show or hide zone dividers with the Show zone dividers option. With this option off, the lines that represent the divisions between zones do not appear on the border.

In Zone Formatting groupbox when Show zone dividers is checked, you can control the line font, line thickness, length for the dividers.

There are also settings under Center zone divider that allow you to control the center zone divider’s length in both directions from the border.

Use Center zone divider settings to control the length of the center zone divider in both directions from the border.

If you do not want center zone divider to extend into the drafting area of your drawing, you can input 0 (zero) into the second field.

Under Zone labels, you will find several options and settings that allow you to control the visibility, placement and font of the letters and numbers which label your zone columns and rows.

Layer

Finally, you can even set a layer upon which your border should be placed within the Layer groupbox.

Ready?

Once you have made all your choices for options and settings on this page of the PropertyManager, you can choose OK button to accept, or you can continue on to the next page for one more advanced function.

Mask Area to Remove some Zone Formatting

Page 3 of the Automatic Border PropertyManager allows you to create one or more masks for your border. A mask is an area on your border where you wish to remove zone labels and dividers. Typically, you will use masks to create space outside your margins to add a company’s legal notice or (if you are still plotting your drawings) you can add part number, sheet number or other information to quickly index through a pile of drawings.

To create a mask, click on the plus sign button.

When you click on the plus sign button, a box will appear on the Sheet Format. You can modify the size and location of this box using the grips.

For example, if you wish to add your company’s copyright notice to the upper left, move and resize the box to cover the upper left corner of your border.

You can add more than one mask. Each mask that you create will appear in the PropertyManager.

All Done!

When you select OK, you accept all the changes that you’ve made to your border, including the masked area. You will still be in the Sheet Format mode. Add any additional details you wish for your Sheet Format.

Return to your drawing’s Sheet mode by selecting Edit Sheet Format one more time.

Your changes will now be the background to your drawing.

If you wish to reuse your newly edited Sheet Format, use the Save Sheet Format command. Find this command in the File pulldown menu, shown above.

Automatic Border tool simplifies a task that can be a tedious sketching exercise. Not only does the above functionality allow you quickly create the drawing border that you want, you can easily edit your drawing border as the need arises.

How to add a Geometric Tolerance frame to your Sheet Format

**OUTDATED Content: Update–>SOLIDWORKS 2020 now allows you to add Geometric Tolerance and Surface Finish symbols onto your Sheet Formats directly without the following workaround**

SolidWorks Sheet Formats do not support Geometric Tolerance frames. So, what can be done if you wish to display a frame with your Sheet Format on drawings?

First, a quick review. SolidWorks has two separate files that serve as the starting point for creating new drawings. The primary file is the Drawing Template (*.slddot). Every time you start a new drawing, it must be from an existing Drawing Template. The template contains all the settings and other information needed for every drawing. In particular, it uses information from a Sheet Format (*.slddrt) for the border and title block. Each time you create a new sheet on your drawing, the Sheet Format is directly loaded. However, neither the Sheet Format or the Drawing Template automatically update existing drawings. For more information on Sheet Formats and Drawing Templates, see SolidWorks Help. The tip found in this article is for more advanced users and CAD Administrators that are already familiar with these topics.

Back to the story. Perhaps your company is moving towards using the model to define your product, but still uses the drawing to established specifications, such as tolerances, general notes, process control dimensions, etc. Common practice for this scenario is to establish a generic Profile specification on the drawing that is then applied to the model. But, you cannot store a Geometric Tolerance frame within a Sheet Format. You won’t likely want to draw your frame using sketches.

Solution? You can have a Sheet Format display a Geometric Tolerance frame that is present on a Drawing Template! Here’s how.

1. First, make backup copies of your Sheet Formats and Drawing Templates! OK, once that is done, open your Drawing Template using File>Open dialog set to Template (*.prtdot; *.asmdot; *.drwdot)

2. Create your Geometric Tolerance frame using the Geometric Tolerance annotation tool.

3. Place your new frame in the lower right corner of your Drawing Template. Don’t be concerned if it overlaps the border, but it is a good idea to keep it inside the paper space.

4. Create an annotation note (Insert>Annotations>Note…) and place it anywhere on the drawing.

5. While the annotation note is still being edited, click on the Geometric Tolerance frame. The frame will now appear in the note. Select OK to accept.

6. Select the new note.

7. Press CTRL-X. The note should disappear, as it is being cut from the Drawing Template.

8. RMB click on any empty area of the blank paper space and select Edit Sheet Format. This will take you into the Sheet Format editing mode.

9. Click on the approximate location where you wish the frame to appear and press CTRL-V. This will insert the note onto the Sheet Format. Click and drag it to the desired location.

10. RMB click on an empty area of the paper space. Select Edit Sheet. This will exit the Sheet Format mode and return you to normal drawing mode.

11. RMB click on the original Geometric Tolerance frame and select Hide.

12. Goto File>Save to save your Drawing Template.

13. Goto File>Save Sheet Format to save your Sheet Format.

(14.) Now, if you wish to edit the frame later, simply use View>Hide/Show Annotations. The hidden frame will appear faded gray. Select it and it will turn black. Press ESC to exit the Hide/Show mode. Edit the frame as your normally would any Geometric Tolerance frame. When done, hide it again. You may need to Rebuild to see the update.

Note: If you open the Sheet Format directly without loading the Drawing Template or if you load the Sheet Format into a drawing created with an older Template, the annotation note containing the frame will be blank. This is because the information is contained in your new Drawing Template, but the note is in the Sheet Format.

Product Review: Template Wizard (2010)

Several years ago, I reviewed one of the earliest versions of Template Wizard, published by 3 Dawn Consulting, LLC at SolidWorksTemplates.com. Template Wizard is an application which fills a gap in SolidWorks functionality by creating the process to automatically generate document templates for drawings, parts and assemblies. Kevin Van Liere of 3 Dawn Consulting has provided to me a new license of Template Wizard for the purpose of this new review. This review is my own content without input of others.

The current version of Template Wizard is refined and more capable. Template Wizard gives the user the ability to create templates from scratch. Users may also create drawing templates from AutoCAD generated files. If the user wishes, they may use it to edit existing SolidWorks drawing templates.

User Interface

Template Wizard is an add-in that runs within the PropertyManager pane inside of SolidWorks. Selecting settings within the interface is similar to other functions that run within the PropertyManager. Users create new templates in a 9 step process. The process starts with a blank drawing sheet and ends with a fully functional templates for drawings, parts and assemblies. When creating a drawing template, some user interaction with the view pane is required to place objects and anchor points.

Installation

Installation is quick and painless. Just execute the downloaded install file, then start up SolidWorks. Template Wizard appears as a pulldown menu. The user will be prompted to enter a registration code (provided at the time of purchase) the first time before they create a new template.

Workflow

If a user wishes to create new templates, it is recommended that they create a drawing template first. As mentioned, Template Wizard takes the user through a series of steps. Once the drawing template is complete, it then allows the user to transfer applicable settings over to new part and assembly templates.

The order of drawing template creation tasks is fairly logical. The user is prompted at each step:

Drawing size, view projection, standards, units of measure, etc.
Border creation, margins, zones, border layer. Although Template Wizard does automatically create borders based on user choices, a nice function to include might have been the ability to choose settings that automatically follow standard ISO or ASME borders, based on drawing size.
Title block and custom properties. Title blocks may be created from existing title blocks or created from scratch using dozens of field blocks. This step is likely the most complex.
Establish tables and their anchors. This one function by itself may make Template Wizard worth its price. SolidWorks has anchors that serve as automatic starting points when the user inserts tables onto a drawing. However, this anchor functionality is somewhat under-documented and hidden. Template Wizard labels each anchor which allows the user to see where and what they are.
Fonts, bent leader length and tangent edge settings.
Save “Page Design”. One thing that I find confusing is the use of alternative terminology in Template Wizard. A page design means sheet format.
Establish the “next sheet” variable and save “template design”. “Next sheet” variable is a quirky SolidWorks setting that establishes the drawing template. Template Wizard uses this variable in a cleaver way to allow drawing templates to utilized a different sheet format for additional sheets of a multi-sheet drawing.
Create part and assembly templates, and the custom properties file. This reduces the effort of creating part and assembly templates down to a push of a button.

Update Wizard

Though I have not tested this functionality, it is important to note that Template Wizard has a function called Update Wizard. This tool gives the user the power to update the sheet format of a whole bunch of drawings at one time. The tool even allows the user to find and replace specific text in the same way!

Purchasing options

Template Wizard is available through the SolidWorksTemplates.com website. Given the value and time-savings potential of Template Wizard, the price of US$295.00 seems reasonable. Visa and MasterCard are accepted for immediate delivery of the software license. Paypal, invoice and check are also excepted.

Findings

Template Wizard was created because SolidWorks does not provide a simple method for template creation. The process in SolidWorks is not well documented nor easily understood by new or some experienced users. Template Wizard allows the user to bypass the learning curve by providing powerful tools in a fairly straightforward process. However, even though Template Wizard is a great tool, it is not completely intuitive.

The user should read Template Wizard’s Help file before using it. Treat the Help file as a tutorial. The Help file gives the user information they need to make certain choices. For example, during the Title Block creation step, the user is presented with tons of choices. Those choices are defined in the Help file under “Pre-Designed Title Blocks” and “Title Block Elements”. I would like to see this information included within the Template Wizard’s workflow in the form of a preview window or something similar.

Where Template Wizard excels is in the fact that it breaks down the template creation process into a series of steps. Many of these steps are wonderfully automated, drastically reducing the time it takes to create a template. It even changes settings in SolidWorks itself to allow the user more flexibility in how they wish to save and use their new templates. As a byproduct of its workflow, Template Wizard also serves as an education tool. It teaches the user about what is needed to make sheet formats and templates in SolidWorks.

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Template Wizard’s value comes from the time and effort saved during the creation of SolidWorks templates. It is not an application that has a high reuse value. However, I do recommend keeping it installed (but inactive) on SolidWorks. This will allow the user to make adjustments to their templates over time, as needs change.

Template Wizard is not for that do-it-yourself person whose independent spirit and drive pushes them to create their own template and sheet formats. It is for the person or company that does not wish to spend a lot time creating, changing or maintaining templates.

Drawing Template with Two Different Sheet Formats (Part 2)

UPDATE for SolidWorks 2014: The following protocol is no longer necessary to achieve a different sheet format for addition sheets on a drawing. Please see 2014 What’s New in SolidWorks – Sheet Formats for current information.

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Here is the [no-longer-necessary] protocol to set up a Drawing Template so that it can use two completely different Sheet Formats without requiring any additional action by the user when they start a new drawing.

This protocol tricks SolidWorks into having a Drawing Template use one Sheet Format for sheet 1, but also to have a different Sheet Format as the default for any added sheets. It does this by swapping around the names of the Sheet Format files.

This allows a CAD Administrator to set up their Drawing Templates to be ASME compliant by automatically calling up the simplified title block when additional sheets are added to a drawing.

Instructions

In Windows Explorer:

1. Save a backup copy of the current sheet 1 and multi-sheet Sheet Format files. Also, save a backup copy of your Drawing Template.

2. Rename multi-sheet file, such as adding an underscore in front of its name. For example, if your multi-sheet file is named “C-SIZE-SECOND.slddrt”, rename it to “_C-SIZE-SECOND.slddrt”.

3. Rename sheet 1 file so that is has the original name of the multi-sheet file. For example, if your sheet 1 file is “C-SIZE.slddrt”, rename it to “C-SIZE-SECOND.slddrt”.

In SolidWorks:

4. Start SolidWorks.

5. Open your Drawing Template.

6. Load your renamed sheet 1 Sheet Format. In the example above, this would be “C-SIZE-SECOND.slddrt”. The result should be a drawing that shows your sheet 1.

7. Save your Drawing Template.

8. Close SolidWorks

In Windows Explorer:

9. Rename sheet 1 to its original name. In the example above, rename the “C-SIZE-SECOND.slddrt” file back to “C-SIZE.slddrt”.

10. Rename your original multi-sheet file to its original name. In the example above, rename “_C-SIZE-SECOND.slddrt” to “C-SIZE-SECOND.slddrt”.

In SolidWorks:

11. Start SolidWorks.

12. Test results by starting a new drawing using the same Drawing Template. Sheet 1 should appear on sheet 1.

13. Create sheet 2. The multi-sheet format should appear on sheet 2.

For best results, uncheck “Show sheet format dialog on add new sheet” in Tools pulldown>Options…>System Options tab>Drawings.

The limitation of this method is when the administrator wishes to change sheet 1 of the Drawing Template, they will have to replicate these steps each time. That doesn’t happen often and well worth the savings in time produced by implementing this method within the Drawing Template.

Additional keywords: 2 title blocks drawing

Drawing Template with Two Different Sheet Formats (Part 1)

A long sought after function in SolidWorks ~~that has gone pretty much ignored~~ is allowing users to set up Drawing Templates with two different Sheet Formats (one for Sheet 1 of X and one for all other X of X sheets). [In the past, m]ost of us just had to directly pick and load the separate X of X sheet when we add a sheet to a drawing.

Some half solutions do did exist to get around the limitation. I have seen one hack that involves using the X of X sheet Sheet Format as the default sheet format with sheet 1 of the Template itself simply having addition entities around the Sheet Format entities to form the complete sheet 1 of X “format”. Another way is was to have two sheets already present in the Drawing Template, each one with its own Sheet Format; then delete sheet 2 when it is not used. No more half steps!

There is a way to have two completely different Sheet Formats embedded into a Drawing Template without having additional sheets already present. I am currently working on writing up the protocol. I will post the steps on Thursday 7/17/08 (Instructions are now available here). The protocol is not complex as far as I can tell. I just wish to thoroughly experiment and test it before posting. Stay tuned. And, if you know of other ways do to this, then please post your methods (or links to them) here so everyone can compare notes. Who knows, maybe someone else has already published something about this I just know I’ve not seen anything in any other online resources, which is why I’m fairly excited about making this method available.

UPDATE for SolidWorks 2014

SolidWorks 2014 now has a second sheet setting in Document Properties. Fancy workarounds are no longer necessary. Please see 2014 What’s New in SolidWorks – Sheet Formats.