Once we have some views which best communicate our form, we need to show the physical size of the elements in that form and, by carefully deciding how we dimension the form, communicate our design intent

Annotation includes all non geometry elements in the engineering drawing including axis, dimensions, notes and tables.

Revisit Design Intent before dimensioning your model

 

Common issues

  • Inappropriate dimensioning methods – see Chain or Datum Dimensioning below
  • Conflicting dimensions or over constraining
  • Always show axis
  • Dimension as diameters where appropriate, not the default radii
  • Don’t show hidden line in GAs or isometric views, but always in part drawings
  • Round up your model dimensions – do you really want an angle of 14.567 degrees?

 

Creating Annotation

 

Axis

Before we can start dimensioning any arcs we need to show axis.

 

Either;

Select an individual view or Ctrl select multiple views

RMB menu > Show Model Annotation

or;

Annotate tab > Annotations > Show Model Annotations  

 

 

In the Show Model Annotations window pick the Model Datums tab (as image above) > select individual axis or use the Tick All button

 

Dimensions 

Annotate tab > Annotations > Dimension – New References  

Creation is similar to creating dimensions in Sketcher

LMB to select the elements, e.g. length of a line, distance between two lines, radius of an arc

MMB to place the dimension – placement can determine which dimension is created, ie. inside or outside angle

Drag the projection lines, dimension lines and dimension text for best clarity

 

Picks

  • pick a straight line to show its length
  • pick two parallel lines to show the distance between them
  • pick two non parallel lines to show the angle between them – MMB pick position for inside or outside angle
  • pick an arc to show its radius
  • pick an arc once, pick it again, then MMB to shows its diameter

Hint:  If a radius or diameter dimension fails or is created with an X and Y element then go back and make sure the plane of the diameter is parallel to the screen – its axis is normal to the screen.  It only has to be a fraction of a degree off parallel and the circle becomes an ellipse.

 

Moving Dimension text

Whilst in the Annotate tab pick on the dimn. text and drag it to position. Hold Shift to give you extra move options particularly when moving radius dimns.

 

Annotation Text Formatting 

Make sure your numbers and text are of a suitable height and font style for maximum clarity.

Either;

Dbl click a dimension or text > Properties > Text Style tab

or;

drag a box around many elements, RMB > Properties > Text Style tab

The defaults are driven by the .dtl config file BS8888.dtl in the working directory

 

Dimension Text

Select dimn > RMB menu > Properties > Properties tab > Name  – this shows the label or name of the dimension (from the model) which is driving the dimension text in the Display tab.  By default you will see @D in the Display text window.  You can simply add text before or after @D to modify the dimension text.

You can control the entire text label by replacing the @D with @O to overwrite the default text.  Put in your own text after the @O

 

Notes

Notes add additional information to the drawing sheet either floating on the sheet or attached to an entity via a leader.

Caution:  if you put dimensional information in a note manually it is not associative to the model – if the model changes you need to remember to manually update the note.  We can exploit the power of the parametric system to link notes to model dimensions.

 

To find a dimension name

  • in the model file RMB menu > Edit on the appropriate feature
  • this will show the dimensions associated with that feature
  • Tools tab > Model Intent > Switch Symbols
  • this is the identity which can be used in notes and dimensions text

 

In the example below, a note to detail the hole is neater then applying the dimensions to the section view.  The note is associated to dimensions in the model.  Insert &[dimn name] (see above) in the Note text box to insert the dimension in your text and remain associative.

 

 

Including parameters in notes or situations when a required parameter doesn’t directly exist

 

Dimensioning to a symmetry plane

If a part is completely symmetrical then you can robustly communicate the design intent and save space by using a half view and dimension from a centre line.

You will need to have a datum plane as the symmetry plane.  RMB > properties for the datum plane in the part file. Rename the plane CL and set to the middle Type setting.  This will allow you to use the plane for dimensioning in the drawing.

Create dimensions in the full view and then change the view to a half view.

 

 

Conflicting dimensions or over constraining

 

This drawings has too many dimensions – changing one dimension will conflict with the others

 

Feature groups

 

2000.dimn.scheme.feature.grps.isoChain or Datum Dimensioning?

Chain

Seems logical and is appropriate for the hole group and the round ended slot but the long chain across the top will suffer from an accumulation of tolerances – with a nominal +/- 0,1mm tolerance and if all the dimensions went +0,1mm then the overall length would be +0,7mm rather than +/-0,1mm

This method also does not capture the design intent – if we increase the 28 dimension then the cut out width and the overall length also increase.

 

Datum

This method of creating all dimension from a single datum has the advantage of isolating all the dimensions and therefore their tolerances.  But this is only really appropriate at a manufacturing stage as it doesn’t capture the design intent and is problematic through the design development stages.

As described above, the two square slots are referenced to the cut out.  With the dimensioning scheme below, if we change the 120 dimension to move the cut out all the other edges will stay where they are and we will have to manually change every dimensions – the design intent is no captured in the dimensioning scheme

 

Dimension the feature group then position the feature group

What we tend to see is a mixture of methods applied to capture the design intent.  Now if we change the 120 dimension the cut out and the slots in the cut out move and maintain their group dimensions.