Working with Sketches (Sketch)

HiCAD distinguishes between (planar) Sketches and 3-D Sketches.

Sketches are 3-D parts which lie in a plane and have free edges.They are, for instance, used for the creation of extruded solids, bores and subtractions, as well as for sweeps and sectional views. Sketches have the part name SKIZZE (SKETCH) and the part type Part with free edges. HiCAD automatically assigns a purpose to planar sketches upon their creation.

A 3-D-Sketch is an aggregation of graphical elements, i.e. of lines and circles, without any references to surfaces. 3-D Sketches are, for instance, used for the generation of surfaces, the definition of points and point grids for freeform geometries, or as guidelines during the placing of cross-sections.The 3-D points of a composite edge are interpreted as support points of curves in the process.

The functions for sketches and 3-D sketches can be found on the Sketch tab.

The purpose of planar sketches

HiCAD automatically assigns a purpose to planar sketches upon their creation. One distinguishes between

• Purpose = Part
• Purpose = Create/Edit

Sketches with the purpose Create/Edit are, in principle, "auxiliary elements" from which other parts, processings and sectional views, detail views or cut-outs. Sketches with this purpose are visualized with broader lines in the active view. They are also visible in shaded models.

Sketches with the purpose Part are regarded as "normal" parts that are used as elements of the drawing. They distinguish themselves from sketches with the purpose Create/Edit as follows:

• In cut-outs, sectional views and detail views the sketch will be cut.
• The sketches have no special representation and are not shown in shaded models (without edges).
• The sketch can be edited with the functions available at 3-D-Standard > Tools > Crossh., i.e. it may contain centre lines, crosshairs etc.

When a new sketch is created, HiCAD automatically determines its purpose. For example, sketches that are created in connection with View functions, during deriving of new 3-D parts from a sketch, during processing of 3-D parts with sketches etc. will obtain the purpose Create/Edit.

In contrast, if a sketch is created with the functions of the Sketch tab, the purpose specified in the Configuration Editor will be assigned. The default setting is Always Create/Edit. This default setting can be changed in the Configuration Editor, at System settings > Sketches.

Purpose for new sketches / new sketches in Metal Engineering grid

This setting determines which purpose will be assigned when a sketch is explicitly created with the functions of the Sketch tab (default: Always Create/Edit). The alternatives are Always part and Always query. If the setting Always query is used, you will be asked to specify the purpose whenever you create a new sketch:

For sketches which have been created via the Metal Engineering plugin the setting setting Always query is not available.

Subsequent changing of the purpose

You have the following options to change the purpose of a sketch:

• On the Sketch tab, choose Tools > Sort GE > Change purpose, or
• Right-click the sketch either in the drawing or in the ICN and select Further > Change purpose .

Please remember that a change of purpose is not possible for sketches which have the purpose Part and contain technical tools.

Sketch representation

Sketch representation for cut-out/sectional/detail view

This setting concerns sketches which were created during the definition of sectional views, detail views and cut-outs. These sketches can either be shown in all views or only in the active view (default).

Sketch representation for creation of new bodies

This setting concerns sketches which were created during the creation of new bodies, e.g. in connection with the Extruded part, Revolved part, C-edge sweep or Sheet from solid function etc. These sketches can either be shown in all views (default) or only in the active view.

Sketch representation for processing of bodies with sketch

This setting concerns sketches which were created during the processing of bodies, e.g. in connection with the Add and Subtract function etc. These sketches can either be shown in all views (default) or only in the active view.

General notes on Sketches

• Sketches as well as 3-D Sketches can be parameterised using the HCM Parametrics tool that enables you to position and displace elements of a sketch or 3-D sketch. For this, the elements of the sketch/3-D sketch are linked together by means of so-called constraints, i.e. dimension relationships, logical relations and restrictions. The parametrics functions transform the corresponding elements in such a way that the defined constraints are fulfilled.
• When polylines are sketched, the corresponding HCM constraints can also be created automatically. The individual elements of the polyline are then automatically linked by means of corresponding dimensional and positional constraints. For this to happen, select Sketches > HCM > Update system > Settings and activate the Enter constraints checkbox in the Sketch area.
• If a part contains sketches with HCM conditions as sub-parts, these dimension conditions can be automatically displayed during identification of the superordinate part. Select Sketches > HCM > Update system > Settings and activate the Dimension sub-sketch checkbox in the General area.
• If HCM constraints are assigned to a sketch, you can highlight these constraints in the drawing by clicking them in the HCM tab of the ICN (or vice versa).
• Right-clicking a sketch opens the context menu for sketches. Here you can find functions enabling you to derive other 3-D parts from the sketch, e.g. extruded parts, revolved parts, beams, plates, gratings etc. If a sketch has been assigned as a sub-part to a 3-D solid, the Add and Subtract functions are also available in the context menu of the sketch. When you call one of these functions via the context menu, the superordinate solid will be processed.
• 3-D Sketches containing HCM constraints are identified in the ICN by a icon.
• When using the Sketch functions, you can press and hold down the CTRL key and the left mouse button to drop the perpendicular from the current cursor position to the nearest line/edge. Please note that in this case the point options that are indicated next to the cursor (e.g.I = End point or M = Mid point), or the sketching grid (e.g. when selecting 2-D Geometry > Draw > Line) will be ignored, i.e. neither the end point nor the displayed grid point will be applied, but always the nearest online point instead.
• If a sketch is cloned, the clones will also take over the usage of the original.
• The creation of sketch lines is not possible while the assembly is active. If an assembly is active, the functions for the creation of sketch elements will be greyed out. This is also the case if a Sheet Metal main part or a multi-part Steel Engineering beam is active. In this way an accidental placing of sketch lines in assemblies will be automatically prevented. An insertion of assembly points and isolated points, however, is possible. Of course, you can still create a new sketch with the functions Sketch and 3-D Sketch while the assembly is active. Please note however that the sketch will then become the active part to which the subsequently line elements will be assigned.

Sketch Functions (3-D)