Example of a Design Variant with Sketch
- Create a drawing with a processing plane and draw a sketch using the function Sketch > New > Create new sketch in plane, as main part
. Parameterize this sketch with the Sketch HCM. A detailed example of creating a sketch with HCM constraints can be found here: Bore Patterns - Example.
Example: Parameterized sketch
- On the Sketch Ribbon, choose New > New point
and assign an isolated point to the sketch. This point will then be parameterized.
Example: Parameterized sketch with fitting point
- Create a cuboid using the 3-D Standard > New > Solid primitive
function, which is to receive a subtraction with the help of the sketch: Create the subtraction by choosing 3-D-Standard > Process with sketch > Subtract part, via translation 
. - Create a processing plane on the base plane of the subtraction and then add a bore grid. To do this, choose 3-D Standard > Standard Processings > Through hole, variable
. - Create a dummy part using the 3-D Standard > New > Dummy part, new
function. Move the cuboid in the ICN under the dummy part and mark the dummy part as a design variant base body by clicking with a right-click in the empty feature log of the dummy part and selecting the option Design variant base body: Yes in the dialogue window that appears. - Enter the variables in the variables table of the dummy part by selecting Parameter variables of variant in the same dialogue window.
- Define the variables.
- In the the feature log of the cuboid below the Subtract... entry, right-click Processing plane and select Edit formula.
- Enter active_coor() into the input mask.
- Right-click the Cuboid in the feature log and select Formula for processed part. Enter the text active_part() ein.
- Right-click in the empty feature log of the Dummy part and select Create design variants. Activate the three dots and enter a name for the design variant. Then choose Save twice.
- Create a new drawing and then create a new standard part, for example. You can now access the design variant iby choosing Drawing > Insert Part > Insert part, via Explorer
.
