DSM V6 - Application of GD&T using Annotation Methods
Summary: An In-Depth Article Model or Drawings for Quick Definitions
This in-depth article will concentrate on 'Annotate' Geometrical Dimensions and Tolerancing (GD&T) for the creation of Feature Control Frames with and without referencing Datums. This may assist the occasional modelling engineer or designer to quickly define features without knowing the procedures required to use the 'Encoded' method.
The alternative method uses 'Encoded' GD&T, a complete logic-based software definition (based on ASME Y14.5 2009) requiring rigorous procedural structured routines to create Feature Control Frames. An illegal definition is prohibited.
A separate article / tutorial will be made on Encoded GD&T use.
Note:
Annotate Geometrical Tolerancing with Feature Control Frames, Datums and Notes, all are placed within an Annotation planes or a Plane. These are created manually with software guidance in the modelling window or on the plane of the drawing sheet by default in the drawing sheet window. The extensive Instructions that follow are provided to create and also copy between modelling and drawing windows if required - it might not be necessary at all!
Annotated GD&T Feature Control Frames are not linked between modelling and drawing views. If necessary, this article tell's you how to easily duplicate the information.
Annotated GD&T could be suitable in early stage design as it's fairly simple to create without having extensive knowledge of DSM or on an unfinished design. Often it's engineering practice to only specify particularly important features for manufacturing and Inspection approval in the early stages, leaving the rest for later specification or unspecified as made to a standard known minimum precision.
It must be stated that, in any GD&T definition, knowledge and application of appropriate principles is a prerequisite.
Chapter headings:
Comments about 'Annotate GD&T' for Feature Control frames
Differences between 'Annotate and Encode' GD&T Feature Control frames
Creation of Feature Control frames > On a Drawing Sheet
Adding Character Symbols inside the Feature Control frame
Attaching the Feature Control Frame to the model feature
Creation of Feature Control frames > On a Model
Notes on the COPYING ANNOTATED GD&T between Models <> Drawings if necessary
PASTING to DRAWING: MODEL CREATED Annotated GD&T Feature Control Frames:
PASTING to MODEL > DRAWING CREATED Annotated GD&T Feature Control Frames:
EXAMPLES of Annotated Geometric tolerancing without a reference Datum:
Displaying a created DATUM in both Modelling and Drawing windows if necessary.
Notes on the MULTIPLE display of GD&T (feature folder) Datums
Notes on Model Annotation Dimensions and the display within a Drawing Sheet view
CAUTION on DIMENSIONING: Importance of 'True View' dimensioning
How to quickly create a drawing, True Projected View from another view
If you want to read in a different order and need to access this list for navigation, click the icon 
Comments about 'Annotate GD&T' for Feature Control Frames
Detail tab > Annotation > Geometrical tolerance > Annotate GD&T
Menu command > Feature Control Frame Feature Control Frame example
Note: Annotate GD&T can be made on either the model or in the Drawing Sheet model views - it's the specifiers choice.
DesignSparks' suggestion is to first decide if a drawing is necessary or could the information be made on the model and supplied by a rsdocx file, a printed .PDF or other image file, perhaps just a screen shot pasted into another document would suffice.
It is expected most users will want to annotate on the drawing, but it's also possible to annotate on the model.
If needed to duplicate a model annotation within it's drawing, either create it again or use the copy and paste methods as described below. Annotated GD&T feature control frames are usually small character sets, but notes may be quite extensive and time-consuming to duplicate. The in-depth and extensive description below will impart all necessary information.
Differences between 'Annotate' and 'Encode' GD&T Feature Control Frames
Annotated Feature Control frames can not be linked or transferred between model to drawing or vice versa. After initial creation, instead, they have to be copied as described below or recreated.
Encoded Feature Control frames (not described in this article) can be transferred between model > drawings and vice versa without copying or duplication and are linked.
See below for an IN-DEPTH description on the creation or copying of Annotated Feature Control Frames and notes, the creation and insertion of special characters into Feature Control Frame dialogue fields.
Study the diagrams below showing the procedure in detail.
Creation of Feature Control Frames
ON A DRAWING SHEET:
Add Annotate GD&T Feature Control Frame
Select the command Annotate GD&T >
This 'Position' symbol is initially shown > 
Place the default 'Position' symbol near to the applicable feature. Change the symbol using the drop-down listing as shown below. Manually complete the Geometrical Tolerance Frame - A partial or completed entry is necessary or the symbol is removed. Later complete or alter the frame contents as necessary at any stage.
Note that all 'Annotations' within a drawing are placed in the plane of the drawing sheet and are owned by the sheet.
For specification, consult the applicable GD&T standard.
Adding Character Symbols inside the Feature Control frame
The inclusion of symbols into the Feature Control frame, such as the Diameter, Maximum Material Condition, Least Material Condition, Projection depth etc, is accomplished by first creating a note and adding the symbol within it.
Consider creating a master note rsdocx file and pasting from that.
To add a symbol into the Feature Control frame, select the note and highlight only the relevant symbol >Ctrl C
Now select the Feature Control Frame >
Place the cursor at the insertion position and paste (Ctrl V) symbol. Repeat for each inserted symbol inserting: 
Drawing Sheet 'Plane' > All annotations, dimensions, notes, feature Control frames, etc are projected onto this plane.
In the Structure Browser, notes and Feature Control frames are added underneath the 'Notes' folder owned by the current Sheet, noted as 
This sheet 'Notes' data is not linked or yet available to the model.
Attaching the Feature Control Frame to the model feature
Attaching the Feature Control frame to a model feature and to a drawing view.
Select Note Leader
Position mouse over Note or Feature Control frame to display all attachment locations - select note attachment position.
Select model attachment position. Arrow style can be changed
Arrow head attaches to the model geometry, it being now not constrained to the drawing sheet plane and also links the Feature Control frame to the drawing view. See the GIF below:
Creation of Feature Control Frames
ON THE MODEL:
Add Annotate GD&T Feature Control Frame
Within the modelling window, open the Detail tab
Select the command Annotate GD&T >
This 'Position' symbol is initially shown >
It is oriented and aligned to either the active annotation plane 
If no Annotation plane / plane exists, an annotation plane is created on the undisplayed world origin xy plane, on any displayed origin axis or on a highlighted model face.
The newly created annotation plane or existing but empty plane icon then changes (green curves added), indicating the plane has contents:
When placing a symbol, if the active Annotation plane is incorrect, right mouse click 'Set new annotation plane' and select within the graphics area a model face, an annotation plane, a dimension, a note, or an Annotation plane from the structure browser. Refer to the GIF below.
With no commands active, the activation of an Annotation plane from within the graphics area is by either selecting the plane boundary >right click> Activate or by simply selecting any note, dimension, or Feature Control frame. Note the Structure browser showing the new activated planes. Refer to the GIF below:
Notes on the COPYING ANNOTATED GD&T between Models <> Drawings if necessary
Annotated GD&T can not be transferred and linked between Model<>Drawing, unlike Encoded GD&T. The following in-depth notes provides guidance and explanations on the necessary steps to copy.
Text notes, special characters such as 
PASTING to DRAWING: MODEL CREATED Annotated GD&T Feature Control Frames:
PASTING to MODEL > DRAWING CREATED Annotated GD&T Feature Control Frames:
EXAMPLES of Annotated Geometric tolerancing without a reference Datum:
On a MODEL, place on a Plane or Annotation plane.
On a DRAWING, automatically placed in the plane of the drawing sheet.
Datums for GD&T definition are not always necessary. Here are some examples: Note the examples may not be to the latest standards official definition. If required to be so, please refer to the applicable standards.
It must be stated that, in any definition, knowledge and application of GD&T principles is a prerequisite which applies equally to the designer and to the manufacturer.
GD&Tolerances may equally be specified for stringent or very loose requirements, where the primary aim is to lower manufacturing costs.
Example of prismatic-sided machined part:
Parallelism >
Flatness >
Angularity >
Squareness >
Example of a cylindrical machined shaft:
Circularity and Cylindricity
Examples of relative positioning:
Slot alignment position to Bore CL - Both, irrespective of feature size.
Slot alignment to the middle of the bar using *Symmetry
The Inner slot Mid plane must be within 0,25 from the mid plane of the end faces.
* Symmetry definition: Symmetry in ASME 2018 has been replaced by using GD&T 'Position'. It however, remains in the ISO GD&T standards.
DATUMS:
Specifying a Datum plane creates or adds a Planar Surface into a GD&T (Feature) folder.
Planar Face datums are specially highlighted in the graphics area upon structure browser mouse proximity for face area clarification and right click options > Delete : Rename : Create Datum Feature symbol
Note GD&T folder and its contents can not be undisplayed - it's symbols are owned in the Annotation plane or planes which can be display controlled.
Adding Datums to a DRAWING
Datums added to faces within drawing views:
Note the following procedure.
Select the command >
Select the applicable face - note the software will only select a 'Face' as shown. Although the cursor is over an edge, is not an allowable selection for a Datum.
In the structure of both the model and drawing (view), a GD&T folder is created with a Planar Surface containing a datum. Selection can be helpful for clarity of understanding.
Repeated datum command operations allocate names in sequential alphabet order A,B and C etc , however renaming is possible in both the model and drawing by selection > Right click > Rename
Changing datum A > B
Multiple Co-Planar Faces that are all to be considered as a single datum, can be ctrl (+) incrementally selected. In the example below, 4x faces defines Datum A. By mouse hovering over the Structure Planar Surface, the feature is shown in black colour for clarity:
Note that when created within a drawing, Datum's, GD&T, dimensions and notes are placed on the plane of the drawing sheet. Annotation planes are not created within drawings.
Adding Datums to a MODEL
Datums added to faces on the model:
From the Detail Tab, select the command > 
Note a Datum symbol is added on a new Annotation plane (to be positioned), or can be snapped and placed on an existing annotation plane or plane if a matching direction is found.
In the gif below, whilst placing Datum C with a new annotation plane, observe both within the model's graphic area and in the structure browser how the annotation plane with dimension 5.0 is ignored, but the existing Annotation Planes of A and B can be dynamically snapped to then becoming active in the structure. A new Planar Surface is added to the GD&T folder.
The GD&T Planar Surface software definition guards against basic operator errors - an existing face datum can not have an additional Planar Surface nor alternative Datum reference applied to it - only a duplicated datum is permitted.
Displaying a created DATUM in both Modelling and Drawing windows if necessary.
A model or drawing created datum is not automatically displayed in either the model or drawing counterpart.
Model window
In the Modelling window, expand the GD&T folder > right click on the Planar Surface datum > Create Datum Feature symbol
Note that to display the symbol, an appropriate aligned Annotation plane ( normal ~ perpendicular to the face) will be created. If a parallel Annotation plane or Plane exists, the symbol may be snapped onto it without a new plane being created.
The images below show the creation of a new Annotation plane during Datum Feature symbol creation.
The image below shows an Annotation Plane normal to the datum surface being added to the active component / document. The symbol is then positioned.
Drawing window
Datums may be have a Created datum shown in any view - choose a drawing view to correctly display the datum on as per GD&T standards.
To delete an incorrectly created or duplicated datum symbol, select it in the graphics area > Keyboard Delete only. Do not delete from the Structure browser.
The datum symbol is placed in the plane of the drawing. It can be selected via any GD&T folder for 'document-wide' right-click commands if necessary.
Any appropriate and multiple drawing views can have the Datum created if it's plane is perpendicular to the Drawing sheet plane. Refer to the image below.
Annotation Planes are a structure browser shown in all drawing views - only parallel Annotation planes to the drawing sheet plane can have their dimensions transferred by using the right mouse button commands Show Dimensions or Show All Dimensions. Oblique to sheet planes (out of plane) will not transfer model annotated dimensions.
How to quickly create a drawing, True Projected View from another view
Drawing sheet non x,y orthogonal true face views can quickly be created (if not already created within the modelling 
Note its face must be perpendicular to the drawing sheet plane for accurate dimensions. See the GIF below of a view creation on the angled face suitable for dimensioning between the 3 holes.
The detailed dimensioning between the 3 holes: (An example of true face - not fully dimensioned)
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