CSWA common mistakes
CSWA · Understand the traps and how to avoid them.
Exiting a sketch while entities are still blue (under defined) and moving straight to the next feature.
New users drag geometry 'close enough' and assume the auto-relations applied while sketching are enough; the status bar reading 'Under Defined' is easy to ignore when the shape already looks right.
What to do instead
Before closing every sketch, read the status bar under the graphics area. If it does not say 'Fully Defined', use Tools > Sketch Tools > Fully Define Sketch, or add driving dimensions plus relations until all entities turn black.
Starting the base sketch floating in the middle of the graphics area instead of anchored to the origin.
The natural instinct is to click where there is empty space; the origin glyph is small and easy to miss, and nothing visibly breaks until mates or drawing views are added later.
What to do instead
Snap the first sketch entity to the origin (corner, midpoint, or centre point) and confirm the Coincident relation icon appears. If it was missed, add a Coincident relation between a sketch point and the origin before exiting.
Adding a dimension to geometry that is already related, producing over-defined (yellow) or conflicting sketches.
Automatic relations are switched on by default, so lines are already horizontal/vertical/coincident; the candidate dimensions them again, and then either accepts the 'would over define' prompt or deletes the wrong relation.
What to do instead
When a sketch turns yellow, open Display/Delete Relations, set the filter to 'Over Defining/Conflicting', and delete the redundant relation or dimension rather than the geometry. Alternatively disable automatic relations for sketches that will be fully dimensioned.
Modelling the whole part in the default IPS template when the exam dimensions are given in millimetres.
The stock new-document template defaults to inch units, and the numeric value typed into the dimension box is accepted without question, so every downstream mass/volume answer is wrong by a large factor.
What to do instead
Before the first dimension, check the unit string in the status bar and set Document Properties > Units to MMGS (or the units stated in the question). Cross-check one known dimension against the drawing before continuing.
Accepting the default Blind end condition on extrudes and cuts instead of the condition the drawing implies.
The Extrude PropertyManager opens on Blind with the previous depth value, and the depth field is the only thing candidates look at; 'Through All' versus 'Up To Next' changes the resulting geometry and volume.
What to do instead
Deliberately open the End Condition dropdown for every extrude/cut and choose Blind (with the stated depth), Through All, or Up To Next/Up To Body based on the drawing. For holes that must break through, confirm the cut exits by rotating the model.
Placing fillets, chamfers, or shells early in the feature tree so that later cuts destroy the edges they reference, causing rebuild errors or lost-reference warnings.
Candidates model in the order features appear on the drawing rather than the order that keeps references stable; a subsequent cut removes the edge and the fillet fails or silently changes.
What to do instead
Add finishing features (fillets, chamfers, shells, drafts) at the end of the tree. Rotate the model before selecting edges in a fillet, use the tangent-propagation option, and press Ctrl+Q after each added feature to catch errors immediately.
Finishing the model without deriving the checked value (mass, volume, or centre of mass) that the multiple-choice answers are based on.
Candidates treat the numeric options as recall or estimation questions and never open Evaluate > Mass Properties, so they guess instead of computing from the model they just built.
What to do instead
After rebuilding, apply the material named in the question via the feature tree's Material node, then use Evaluate > Mass Properties and compare mass/volume/centre-of-mass directly against the option list before selecting an answer.
Over-mating or under-mating inserted components - stacking redundant mates until the assembly reports over-defined, or leaving parts free to float.
Candidates add mates until the part 'looks right' on screen, not until its degrees of freedom are removed; a drag test is never performed, so remaining translation or rotation goes unnoticed.
What to do instead
After mating, drag each component in several directions - it should not move. If an over-defined error appears, use MateXpert or the Analyse tab to find the redundant mate, and prefer one well-chosen mate pair (Concentric + Coincident) over several coincident faces.
Inserting components without controlling the first one, so the assembly sits at a random orientation and mass properties/positions do not match the expected answer.
Candidates assume every part should be floating and start adding mates before checking the tree; the first component is fixed by default but subsequent ones inherit the orientation they had when saved.
What to do instead
Verify the first component shows the (f) prefix in the FeatureManager and leave it fixed as the datum. Orient it to the standard view before inserting the rest, and use Move Component with collision detection off to place parts roughly before mating.
Creating drawing views at whatever scale appears automatically and omitting the required section, detail, or isometric view called for by the question.
Insert > Drawing View drops in a view at the sheet's default scale and candidates stop once the geometry is legible, without re-reading the list of views and scale the task specifies.
What to do instead
Set the sheet scale explicitly in Sheet Properties, then build the view set from the question's wording (front/top/right, isometric, section, detail, broken-out). Use Insert > Model Items to pull model dimensions into the views rather than sketching dimensions over them.