On this page:

Stand alone or Internal Sketches

Viewing the Sketchplane

To modify a sketch

Sketch References

Sketch Orientation

Good Sketching

 

 

Sketches are at the root of so much of our core geometry in the CAD environment.  A thorough understanding of how to build a robust sketch which captures design intent and modifies efficiently is essential to good modelling.

 

Stand alone or Internal Sketches

Sketches can be stand alone features in the 3D environment as simple construction geomerty or to drive 3D solid or surface features or internal to a feature.

Stand alone sketch feature

Pros

  • required by some features ie. trajectories, surface structure
  • easy to visualise a volume before it’s built
  • if you delete the feature you don’t lose the driving geometry

Cons

  • additional model tree feature
  • not context sensitive ie. internal axis for revolve, analysis tools

Select a Datum Plane or planar surface.  For a solid surface, select the solid then the surface on the solid.

Activate the  sketch tool

 

Internal sketch feature

Pros

  • reduces model tree
  • is grouped with associated feature in model tree
  • is context sensitive ie. internal axis for revolve, analysis tools

Cons

  • delete the feature, lose the sketch
  • can’t be used to build other features

Select a Datum Plane or planar surface.  For a solid surface, select the solid then the surface on the solid.

Activate the feature tool.  This takes you directly to the sketching environment.

 

Viewing the Sketchplane

By default the model stays in its current position whilst you are sketching.  It is sometimes useful to align the sketchplane parallel to the screen whilst sketching

Choose the Sketch View icon from the Sketch tab or the quick access toolbar

To modify a sketch

Either;

In the graphics area – Dbl click the feature.  Dragable elements have a white triangular cursor.

or;

Select the feature in the grahics area > RMB > Edit Definition

RMB the feature in the model tree (no need to select first) > Edit Definition

Sketch References

All parametric geometry has to be fully explained in relation to the 3D Cartesian coordinate system – the x, y, z dimensions.

The position of your 2D sketch on its sketchplane needs to be described in x and y with dimensions and geometric constraints.  Sketching References are the entities from which dimensions will start and to which geometric relationships are made. These can be assigned before creating constraints and dimensions or whilst creating them.

The software will generally assign some arbitary references and most times these will do, but as your modelling becomes more considered and more complex you will need to choose more appropriate references which properly capture your design intent.

 

 

A coordinate system, point or perpendicular axis can be chosen alone and will generate both vertical and horizontal dimensions.  Otherwise choose a vertical and a horizontal perpendicular plane (surface or datum plane) – choosing edges can be problematic.

 


 

Sketch Orientation

The horizontal x and vertical y vectors within a sketch are arbitarily defined and will generally not be problematic.  But if you say, you sketch on a surface which is not aligned to the dominant model horizontal/vertical and your geometry is therefore in the wrong orientation then you may wish to choose a reference to define you xy vectors.

Choose a planar reference perpendicular to the sketch plane

 

 

Good Sketching

  • Curves [to scale]
  • Geometric Constraints
  • Create Dimensions
  • Modify Dimensions

Creating a robust and successful sketch as the basis of most of the common ProE features is a crucial step on the way to a successful model.

Step 1:  Use the sketcher grid and zoom in/out to make the graphics area the same size as your intended sketch.

This will avoid problematic ‘bit by bit’ scaling through modification of dimensions in the sketch once it is completed.  Large movements of entities will often result in extreme distortion of the sketch.

Step 2:  Using Lines and Arcs (rather than trimmed Circles and Squares) starting from one point and create the sketch in a continuous line.

Trimming circles and squares can often result in end points becoming disconnected so causing open loops which are hard to solve.  You are also more likely to create lines on top of lines – very hard to track down.  Starting from one point and switching from line to arc as you work around the loop will ensure good connection.

Step 3:  Create the sketch to the correct proportions.

This will avoid lots of resizing work.  Drag points and entities to approximately reshape the geometry.

Step 4:  Apply geometric constraints.

Connect the sketch  to the sketching references and use geometric constraints before dimensional constraints to fix its shape and proportions.  This will minimise the number of dimensional constraints. The common constraints you will use are Tangency and Coincidence.

Step 5:  Apply dimensional constraints.

It is good practise to try and leave the sketch with no grey, weak dimensions.  This ensures all dimensions have been considered and checked.

Step 6:  Modify the dimensions.

Using the pick icon, simply double click a dimension to modify it.  Also, using the pick icon you can drag a box around all of your dimensions to select them and then pick the modify icon to list all the dimensions for easy modification. Uncheck the regenerate option as this may cause distortion as each dimension will be updated as you make changes.

Step 7:  Resolve sketch failures.

If the sketch fails it is most commonly due to either disconnection between points causing an open loop – look for weak dimensions of zero – or because you have lines on top of lines – very hard to find.  This last issue is the main advantage to creating the sketched loop an entity at a time continuing from the end point of the previous entity using line and arc segments

 

Round up/down your dimensions

Do you really want your part 47.63mm wide or 42.97degs?  Remember, these dimensions will migrate to your engineering drawings.

 

This method of creating robust sketches is by no means the only way, there are always exceptions everyone develops their own techniques but I have found it to be a good starting point.

 

Interrogating your sketch

For a solid feature your sketch needs to be either;

– a single closed loop

– multiple closed loops which do not overlap

 

Common issues which cause a sketch to fail are;

Tags

 

Usually through bad trimming.  Look for unexplained dimensions.

 

Line on line

 

One line exactly overlapping another is seen as another [incomplete] loop.  Usually through bad trimming. Tricky to find.  Look for unexplained dimensions.

 

Disconnected endpoint

Endpoints seem to join but don’t have appropriate constraints.  This can happen when using the copy edge function.

 

Section Analysis Tools

With both internal and stand alone sketches, the system can use a range of tools to highlight issues with your sketch.