l´m using sketcher every day as many of us. Don´t think my work is top productive.
So my question is simply: What tips, tricks or hotkeay are you using in SKETCHER MODE?
- press SHIFT button and drag the line to make it concident with reference
Every ideas or links are welcome
Thanks in advice
While in the sketch command hitting the RMB has many functions that is not available directly like locking the constraints, lengths, and many more.
I love the power of Creo sketches.
Be careful with splines! They take some care to make them symmetrical. Know you can control curvature start/end angles. Use arc length dimensions instead of perimeter if possible. You can only have one perimeter dimension in each sketch.
Do your geometry math with geometry. This is old world where people use to sketch many views on one sheet to get geometric relationships.
In sketcher, you can do the same thing. Simple example is drawing a quick hex reference to pick off the 30 degree chamfer along the edge of a nut, for instance.
Variable section sweeps require special rules in order to make them variable. 1. Do not project existing geometry. 2. Careful for horizontal/vertical constraints. 3. Test rotation features.
Antonius Dirriwachter wrote:
... Do your geometry math with geometry. ...
Yes! I make liberal use of construction line segments or circles to eliminate duplicate dims that are equal. With the ability now to apply an equal constraint to dims (added in Creo 1 or 2 I think), that isn't as needed.
The concept remains, however, don't have two or more dims in your sketch that need to remain equal that aren't somehow constrained as such.
I also force my dimensions to lock making dragging the remaining freedom at will without loosing constrained geometry.
Know that you can set dimensions as equal using constraints.
Obvious... click a circle twice for diameter or right click and change to diameter
Revolve diameters: 1. use geometry centerlines (datum) and solver will give you recommended diameters. 2. use reference centerlines and click the line/vertex, the centerline, and the same line/vertex to get the diameter dimension.
Shift to disable solver while creating geometry.
If you need to add a reference while sketching, you can press Alt + select the needed reference then continue sketching
I also noticed yesterday something. If you select multiple arcs or circles, you can right click and select equal and all the selection will have the same dimension.
Actually, you don't even need to add references. Sketch the line, then when adding dims or constraints you can pick the new reference directly.
You can build relations in the sketch on the fly by typing the equation in the dimension. I use "sd1/2" often to create symmetry while being able to display both dimensions on the print.
l like your idea:
Just to make it clear --- H & V means Horizontal and Vertical?
Milan Bonka wrote:
... Just to make it clear --- H & V means Horizontal and Vertical?
Creo likes H & V constraints, applies them liberally.