How to add a Geometric Tolerance frame to your Sheet Format

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.

GD&T Feature Control Frame user interface?

Remember this old faithful interface for creating Geometric Tolerance frames (a.k.a, GD&T feature control frames, or GTOL annotations)?

There a new thread on the Drawings forum at SolidWorks Forums asking about how you use this user interface to create Geometric Tolerance Frames.  Your input is very welcome there (and here, if you wish).  What would you do to improve the inferface?

  • When do you use it?
  • How does it work for you?
  • What do you think about the workflow of creating the frame before you place
    it on the sheet?
  • How do you feel about the preview window (and would it be necessary if you
    could just see your frame being modified directly on the sheet)?
  • Do the restrictions within the interface (meant to force you to follow
    GD&T rules) ever prevent you from creating the frame that you need?
  • Have you used the PropertyManager settings that also pop up when you edit an
    existing frame?

ADDA’s Annual Technical & Educational Conference

The American Design Drafting Association (ADDA) is hosting its 52nd Annual Technical & Educational Conference in Kansas City, MO on April 12-15, 2011.  ADDA is heavily focused on the professions of drafting, design, and graphics.  ADDA has a certification program for drafters (mechanical and architectural), civil design drafters, design technicians, and digital designers (which include imaging and editing).  Not everyone has heard of ADDA, and that may be intentional.  Olen Parker, Executive Director, states,

It [ADDA] is small, yet sets the stage for many changes within the profession.  We don’t make noise, we don’t promote ourselves, we are the best kept secret in the profession.  ADDA is very involved in the standards and regulations related to our industry.

Best kept secret?  Well, maybe not anymore. 🙂  Parker also mentioned that ADDA made final reviews to ASME Y14.5-2009, and has members that are involved in a number of national committees and organizations.

The conference

This year’s Annual Technical & Educational Conference will have sessions that cover ASME and GD&T fundamentals, CAD and drawing standards, building codes, graphics, etc.  In particular, they will have sessions for CAD and graphic art applications such as PhotoShop, SolidWorks, Pro/E, AutoCAD, Revit, Sketch-Up, Illustrator, and several others.  Other sessions of note will discuss sustainability, BIM, and even workplace ethics. 

I’m also presenting a talk on establishing company CAD procedures at this year’s conference.  Though this presentation will be similar to my breakout session at SolidWorks World 2011, it will be more applicable to the broader audience at the Annual Technical & Educational Conference.

I will write about many aspects of this conference on SolidWorks Legion, including special attention to the quality and depth of several presentations.  I also hope to have a least a couple of interviews.  I also plan to post tweets on hashtag #atec11 during the event.

This will be my first year attending ADDA’s Annual Technical & Educational Conference, though I’ve been looking for an opportunity for several years.  Please note that ADDA is non-profit.  Although ADDA is giving me full conference access (including some meals) at no cost, I am sorta earning my keep by being one of the presenters.  I am personally paying for all other costs associated with my attendance, including airfare and hotel.

If you are interested in the ADDA, their certification process, or the Annual Technical & Educational Conference, please visit their website for further details.

How to dimension feature patterns on drawings

A couple of days ago, I briefly covered the mythical specification “non-accumulative tolerance” (or “non-cumulative”) as it is often applied to direct dimensions on feature patterns.  See the example in Figure 1 where the dimensional callout attempts to simply dimension a pattern without considering tolerance stack-up.  However, this attempt fails since any two non-adjecent holes cannot avoid accumulation of tolerance due to the dimensioning scheme.  The problem gets worse if three or more positions within the patten are compared to each other.

Non-accumulative tolerance dimension on a pattern
Figure 1

ASME repetitive feature dimensioning scheme

ASME Y14.5-2009 actually provides a linear method to detail feature patterns, called repetitive features and dimensions.  See Figure 2. Unfortunately, the standard does not provide any tolerance rules for its prescribed scheme. Presumably, this leads us to interpret a repetitive feature dimension as though it is shorthand for chain dimensioning.  Chain dimensioning accumulates tolerance as the pattern departs from the dimensioned start position.  Sometimes this is OK, but often this is unacceptable since the accumulation of tolerance can quickly lead to features that do not align to mating features on other components.

Figure 2
Figure 2

Disorganized direct dimensions

Another dimensioning scheme that I’ve seen involves a complete disregard for the fact that a pattern exists.  See Figure 3.  Directly dimensioning each of the positions within the pattern to each other may be acceptable in some scenarios, but likely isn’t a very clear choice for larger feature patterns.  The problem with this scheme is that it can be very difficult to determine the true accumulation of the tolerance stack-up.  It may also be difficult to determine design intent.

Figure 3
Figure 3

Baseline dimension scheme

To avoid the issues associated with other direct dimensioning schemes, one may choose to use baseline dimensioning, which may also be called rectangular coordinate dimensioning in some scenarios.  The advantage of a baseline dimension scheme is that it limits the accumulation of tolerances to the stake-up from just two dimensions.  This is because the total stack-up between any two positions within the feature pattern are related through a common baseline.  The problem with baseline dimensioning is obvious in Figure 4; its take up a lot of space on the drawing.

Figure 4
Figure 4

Ordinate dimensioning

A common alternative to baseline dimensioning is ordinate dimensioning, also known as rectangular coordinate dimensioning without dimension lines.  This scheme also relies on a baseline, referred to as zero (0), from which all of the features are dimensioned.  The advantage of ordinate dimensioning is that it takes up far less space on a drawing, as shown in Figure 5.  Tolerance stack-up is limited to just two dimensions between any two positions within the pattern.

Figure 5
Figure 5

Using GD&T for best results

The best way to avoid accumulation of tolerances is to use a methodology that does not rely on any form of direct dimensions.  ASME Y14.5-2009 actually suggests that GD&T should be used instead of direct dimensions to locate features.  I have discovered the hard way that many individuals in the engineering field have an irrational fear of GD&T.  Even still, GD&T provides a far superior method for the location of positions within a feature pattern. The example in Figure 6 shows a less cluttered drawing.  With the addition of MMC to the feature control frame, this method could provide even better results since it would make use of bonus tolerance.  The position of each feature within the pattern has an optimal tolerance zone that more closely matches design intent.  One more added benefit is that all features controlled by a signal feature control frame are automatically considered as a pattern.

Using GD&T to locate features
Figure 6

Since the tolerance zone is optimized, using GD&T may help reduce costs by allowing the manufacturing process to vary in a way that is more in line with design intent.  In turn, this can reduce the number of unnecessary part rejections.

Conclusion

When detailing feature patterns, one may wish to avoid the use of direct dimensioning methods or shortcuts like the mythical “non-accumulative tolerance”.  The best choice to detail a feature pattern is GD&T.  However, if GD&T is not desired, the next best method is prolly an ordinate dimension scheme.  It should be noted that for each of the dimensioning and tolerancing schemes shown within this article, there are a variety of ways to implement them.  This article is meant to present general examples.  Actual tolerancing requirements are guided by design intent and other considerations per individual cases.




Datum Changes in ASME Y14.5-2009

The following is posted with the permission of the author, David DeLong, who is a ASME GD&T Professional (GDTP) at Quality Management Services, Inc.

Datum Changes to ASME Y14.5 – 2009

Under ASME Y14.5-2009, Maximum Material Condition (MMC) can now apply to datums that are features of size and also surfaces. The 94 standard would only allow MMC on datums that were features of size and NOT surfaces.

A feature of size is a hole or pin of any shape and also a width. In most cases in GD&T, the holes or pins are most important to assembly and are used a great deal as secondary and tertiary datums. Usually, the perimeter of a non-cylindrical part is not functionally important. There are certain cases where there may be a partial hole or cutout that is used in assembly and could now be referenced as a datum.


Maximum Material Boundary

The Maximum Material Boundary (MMB) is a new term used in the 2009 standard and replaces the terms “Maximum Material Condition” and also “Virtual Condition Size” when referring to a datums referenced with the maximum material condition symbol.

In certain cases, MMB is the maximum material size while in other situations, it is the virtual condition size. It depends upon whether the datum is a primary, secondary or tertiary datum.


Let’s review the MMB for datum G in the above example.

If datum G was referenced as a primary datum, the MMB would be the MMC size of the hole which would be the smallest allowable size of the 12 mm hole which is 11.6 mm. It does not make any difference whether or not the feature actually has a virtual condition size as shown, the MMB is still 11.6 mm..

In our example, datum G is referenced at MMC as a secondary datum so the MMB is 12 – 0.4 – 0.2 = 11.4 mm which is the virtual condition size of the hole. If the secondary datum did not have a virtual condition size, it would default to its maximum material condition size of 11.6.

Datum H Reviewed 

If datum H was referenced as a primary datum, the MMB would be its maximum material condition size or smallest allowable size – 8.6 mm.

If datum H was referenced as a secondary datum, the MMB would be its virtual condition size but, in our situation, we have two (2) virtual condition sizes.


The positional tolerance shown would give us a virtual condition diametrical tolerance zone size of 9 – 0.4 (MMC) – 0.3 (perpendicularity) = 8.3 mm.

We also have a refinement of the positional tolerance with a perpendicularity requirement. In this situation, we have a virtual condition size of 9 – 0.4 (MMC) – 0.2 (perpendicularity) = 8.4 mm.

So, if datum H was referenced as a secondary datum, one would use the perpendicularity refinement resulting in a MMB of  9 – 0.4 – 0.2 (perpendicularity) = 8.4 mm.


In our situation, datum H is a tertiary datum and only used for orienting (anti-rotation) the part about datum G so that we are able to confirm all the dimensions. In our situation, we will use the MMB of 9 – 0.4 – 0.3 (positional) = 8.3 mm which includes the positional tolerances rather than its refinement of a perpendicular tolerance.
Here we have 4 holes of 8 +/- 0.3 mm. The feature control frame reflects a positional tolerance of a diametrical tolerance zone of 0.25 mm beyond the MMC referencing primary datum A (usually the mounting surface), secondary datum G at MMC (12 mm hole) and tertiary datum H also at MMC (9 mm hole).


We have already discussed that fact that the MMB changes depending upon whether it is a primary, secondary or tertiary datum. If there is any doubt about the MMB, one can reflect the actual MMB size in the feature control frame as shown above using brackets about the MMB size. This method can also be used if MMB size differs from the calculated size.

Let’s say we wanted the MMB size of datum H to be its refinement size of 8.4. One would then replace the 8.3 in the feature control frame with the refined size of 8.4 and that superseded the calculated MMB size.

For further details, please see the full article at Datums 2009.

It’s All Over!

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.