The binding of sketch's lines is now seen more illustratively
When you add constraints to sketch, lines are marked with the following colors: (MEC-8406)
- Black. When a line and it's points are fully defined .
- Dark purple. When the other end of a line or the center of a circle or arc has been defined .
- Light purple. When a line position is not fixed, even though the line has some constraints like the length, angle, tangent, etc.
- Red. When a line is overdefined.
- Blue. When a line is copied from another part or earlier phase of a part.
- Grey. When a line does not belong in this sketch.
Note: The colors are not displayed if the feature "Draw only wire frame as default" is active.
List of constraints indicates the validity on the constraint
Red text on red background => The constraint is not valid.
Red text => The constraint is in conflict with another constraint, but it is valid.
Black text => The constraint is valid.
The program indicates when the sketch is fully defined
- Message disappears after a short time.
- Or click OK to close the message.
- You can adjust the notification time with user/SETUP-keyword
set.welldefinedmessage.time = 800
- Time is set in milliseconds ()
Curve length is shown now like radius constraint.
Dimension has a prefix "L" ()
When sketching, insert coordinates with keyboard to add automatic dimensions
You save time if you add certain points with keyboard instead of clicking them when sketching. ()
When inserting the coordinates with keyboard, the following constraints are created:
- The end point of straight line => Horizontal and vertical distance constraints.
- A peripheral point of circle => Diameter constraints
- The arc (center point and two peripheral points) the first point on the peripheral => Radius.
- The arc (center point and two peripheral points) the first and second point on the peripheral => Radius and distance constraints
- Second and third ellipse point => Both the radius constraints.
- Two point Rectangle => Both the distance constraints.
- Tree point Rectangle => Distance to the first line, if defining the second point with keyboard. The distance to the second point, if defining the third point.
Adding chamfers or rounds keeps previously made dimensions
Vertex G4 adds quidelines to the deleted section of a line and connects the dimensions to these line endpoints. (MEC-8282)
Better visibility of the Mini Toolbar when you add the arc
A mini-toolbar is used to manage e.g. drawing the three-point arc (tangentially or not). Now the toolbar will appear (in the sketch and the drawing) and re-appear when the cursor stops for a moment.(MEC-7446)
A reference line helps to detect the center point
When the cursor is pointing to a circle or an arc, a reference line is drawn between the cursor and the center point . This applies to sketching or dimensioning a line. (MEC-8148)
- Now it is easier to see whether the arc/circle or the center point is going to be selected.
- This applies to both the drawing and the sketch.
Change the direction of a locked line's reference line
By default, the reference line is drawn in the perpendicular direction to the locked line.
The shortcut key J works now also in 2D and 3D sketches, while it previously worked only in the 2D drawing. (MEC-8148)
The overlapping lines and the intersection of the lines are now displayed graphically
The overlapping lines and the intersection of the lines may prevent or cause problems when extruding or revolving . Now they are illustrated with purple rounds, so that you can detect these flaws easier. (MEC-8107)
Coordinates of a 2D Sketch are now seen more illustratively
Previously, the coordinates that were shown were the coordinates of a model. Now the coordinates are shown as in 2D Drawing to increase their usability. (VX-4719)
Sketching by entering the dimensions is easier than ever
If you are used to sketching by entering the dimensions of the lines, you might have noticed that the last point coordinates are not considered as the relative origon when you change the line functions. For example from the "Two-point line" to the "Circle with a Center and a Radius point". (MEC-8494)
- Now changing the function no longer changes the relative coordinates.
- You can enter the starting point of a new line or the center of the circle directly after you change the line tool relative to the last point of the previous line. There is no need to reset the relative origin with shortcut key Q to the previous line end point.
Spline curve management is easier using the tangent handles
There are guiding lines in the ends of a spline line. They control the shape of the curve . A curve contains also interpolation points. You can add guiding lines ( we call them "Handles") also in these points. The shape of the curve can be controlled with points or guide lines (handles).
Spline curve curvature can be examined visually
The tool is for visually examining the change in curvature's steepness.
You can select the Visualization Settings from the same menu.
You can use function "Trim line to another line" ()also with open spline line. Function "Delete Section of Line" works with open spline curve.
- Trimming into a spline curve is not possible.
- The closed spline line cannot be cut in order to create an open spline line.
- The spline line can be used to modify other lines with a function "Delete Section of Line".