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**OUTDATED Content: Update–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.

It’s All Over!

When “All Over” is applied to a Profile of a Surface, it pretty much defines the entire shape of a part in every direction.

ASME Y14.5M-2009 has been out for a little while now (after almost a year’s delay).  There are significant improvements and clarifications.  One addition in particular caught my attention, the ALL OVER symbol.  When applied to a Profile of a Surface, it pretty much defines the entire shape of a part in every direction (not just ALL AROUND which applies to the profile of a surface along a particular plane).

The symbol is either a double circle at the vertex of the associated bent leader, or the words ALL OVER placed immediately below the feature control frame.

ALL OVER symbols

The symbol indicates that a profile tolerance or other specification shall apply all over the three-dimensional profile of a part. It is applied as “unless otherwise specified” to allow for other existing dimensions and tolerances to take precedence.

ASME Example

The advantage of using this symbol is that it provides control of surfaces over an entire part without regard to part orientation, thus allowing us to directly reference the CAD model as basic and fully controlled, while still detailing critical dimensions and tolerances.  This may help companies better parts where they rely on the CAD model to provide complete specification.  In fact, where a CAD model is declared basic, companies may be able to effectively place the Profile of a Surface FCF with the ALL OVER symbol right into their drawing title blocks along side other tolerancing information.

Model Based Definition (MBD)

As we move further into the realm of 3D CAD software, something that is still catching on is the idea of driving all specifications directly from the model file, instead of having a separate drawing.  There are various terms for this, but I’ve seen Model Based Definition (MBD) most recently.  I personally am not critical of this idea.  I am critical of moving 100% to this form of documentation without better support from our 3D CAD packages and ASME/ISO standards.

Models are generally considered basic.  All this means is that the tolerance is derived from some “other” specification.  This is normally in the form of associated Geometric Tolerances. To fully define a part in MBD, you’ll need a GD&T scheme, often supplemented by traditionally dimensioning and tolerancing where needed.  The difference is that if drawings are not used, this has to be done within the model itself and then is somehow communicated to the manufacturer.  The task to communicate this information to the manufacturer via the model is harder than it might seem as first glance.  This is due to the myriad of 3D CAD formats and versions now available.  GD&T information may not translate to other formats, such as STEP and IGES. 

Additionally, any information that would’ve appeared on the drawings now has to appear within the model itself.  So, shortcutting the drawing step doesn’t mean one gets to ignore the information that would’ve been included on a drawing. It just means all of that now needs to appear in the model.

With that said, ASME Y14.41 supposedly standardizes this effort.  In my opinion (and yes I’ve read it and “own” a copy), it is lacking right now.

If considering a MBD program, just make sure everyone understands that the model is now the drawing; and that means it will need to be as accurately detailed as the drawing would’ve been; and since this information is now in the model, a method of communication will have to be established with the manufacturer if they don’t have the ability to use the format where the GD&T information resides. 

An alternative is to use the drawing in conjuction with the model, which together provide the complete specification.  In this case, the drawing will still be the primary specification (usually for critical-to-function specifications), but it makes use model to complete the specificaiton.  The model can either be basic, or used with some traditional tolerance.  Where the model is basic, I’ve seen companies place a generic profile feature control frame in the general notes.  This FCF is applied to the model for any dimensions that are unspecified on the drawing.  If such as system is employed, it is important to clearly state this on the drawing to prevent ambiguities.