Engineering Drawings

Design & Tech CAD

Engineering drawings – detailing

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’

Capturing design intent – feature dimensions and feature position

Consider the above image. If I was communicating this part to a third party part of my description would describe a rectangular pad in the middle of the angled surface and two holes drilled into the rectangular pad.

The rectangular pad is a feature [not a ProE feature] and the holes in the pad are a feature. Each of these features have their own dimensions to describe them and then dimensions which place them relative to their parent feature. Feature dimensions and feature position.

The pad is placed on the angled face a distance from the side wall and a distance from the bottom edge. It is then x wide and y high. If its position changes I don't want its size to change.

The holes are x and y distances from the edges of the pad. If the pad moves the holes need to stay in the same place on the pad.

These two last statements are my Design Intent. This design intent needs to be captured in my dimensioning scheme.

BAD

Consider the above dimensioning scheme. What would happen if I changed the 7 and 8 dimensions to move the pad down and across slightly?

The pad size would change and the holes would move relative to the pad.

The above scheme will also cause tolerance accumulation. Say I have a general tolerance of
+/- 0.1. The pad width is controlled by the 7 and 39 dimns. Therefore if the 7 was minus and the 39 was plus [or visa versa] the pad feature width is +/- 0.2

BETTER

The above dimensioning scheme better captures my design intent. If I change the 7 and 8 dimensions to move the pad, the pad size will remain constant and the holes will remain in the same place relative to the pad.

The above scheme still does not address what seems to be a symmetrical design intent or the holes centres. In this situation we could dimension from a datum plane which would maintain the holes centres and their position relative to the pad.

Rule: Dimension the feature and position the feature

Conflicting dimensions or over constraining

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

Apply all the same rules from your manual drawing practice - some common issues are:

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
accepting what your given by the CAD - don't be lazy!
nonsense dimensions - see Design Intent

Axis

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

Select an individual view or Ctrl select multiple views

RMB menu > Show Model Annotation > pick the Axis tab > select individual axis or use the Tick All button

Show Model Annotation icon in the Annotation menu will also access this window

Driven Dimensions

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.

Dimension Text

Formatting Dimensions

Make sure your dimension are a suitable height and font style for maximum clarity.

Either; pick the individual dimension, RMB > Properties > Text Style tab

Or; drag a box around all the dimensions, RMB > Properties > Text Style tab

The Defaults are driven by the .dtl config file - in our case, BS8888.dtl in the working directory

Select dimn. > RMB menu > Dimension Properties > Properties > Name - this shows 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 > Edit on the appropriate feature - this will show the dimension associated with that feature. From the Info drop down menu > Switch Dimensions to show the dimensions name rather than value. 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.

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 and dimension from a centre line.

You will need to have a datum plane as the symmetry plane. Right click and properties for the 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 the dimension in the full view and then change the view to a half view.