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- Creo Modeling Questions
- Sketcher - tips, tricks and hotkeys

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Jun 29, 2016
01:00 AM

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Jun 29, 2016
01:00 AM

Sketcher - tips, tricks and hotkeys

Hello,

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? **

**Example: **

- press SHIFT button and drag the line to make it concident with reference

Every ideas or links are welcome

Thanks in advice

Milan Bonka

15 REPLIES 15

Jun 29, 2016
01:15 AM

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Jun 29, 2016
01:15 AM

- You need to hold CTRL to snap to corners or other sketch entities
- select dimension(s) and Control+T will make the dimension strong.
- Select the sketch lines and press Control+G to make them Construction.

Jun 29, 2016
02:13 AM

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Jun 29, 2016
02:13 AM

While in the sketch command hitting the RMB has many functions that is not available directly like locking the constraints, lengths, and many more.

Jun 29, 2016
02:22 AM

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Jun 29, 2016
02:22 AM

Parametric sketches in models or the sketch tool in drawings, symbols, and formats?

Jun 29, 2016
03:10 AM

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Jun 29, 2016
03:10 AM

Parametric sketches in models...

Jun 29, 2016
11:07 AM

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Jun 29, 2016
11:07 AM

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.

Jun 29, 2016
11:16 AM

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Jun 29, 2016
11:16 AM

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.

Jun 29, 2016
11:17 AM

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Jun 29, 2016
11:17 AM

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.

Jun 29, 2016
11:32 AM

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Jun 29, 2016
11:32 AM

Jun 29, 2016
07:55 AM

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Jun 29, 2016
07:55 AM

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.

Jun 29, 2016
09:30 AM

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Jun 29, 2016
09:30 AM

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.

Jun 29, 2016
10:22 AM

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Jun 29, 2016
10:22 AM

Same for lines...

**For example:**

Sketch 5 lines - press RMB - select equal ---> all lines have the same lenght

Jun 29, 2016
08:31 AM

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Jun 29, 2016
08:31 AM

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.

There is always more to learn in Creo.

Jun 29, 2016
09:42 AM

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Jun 29, 2016
09:42 AM

- Be mindful of your sketcher reference plane. Not only does it allow you to control what H & V is, Creo will frequently pick a model surface rather than one of the default datums, creating another unnecessary parent child relationship.
- Always use surfaces for references rather than edges where possible. They are much more robust.
- Get the right number and type of entities in when sketching, don't worry about placing them where they need to go. In fact, I deliberately put them in the wrong place to avoid Creo assuming they should be aligned with something.
- Add "sketcher_starts_in_3D no" to your config to keep the model in 3D while sketching. Makes selecting references easier, especially when trying to pick surfaces vs. edges (see previous bullet)
- Don't worry about picking sketcher references ahead of time. Sketch first, then tie things to model geometry after. It gives you more control over the constraints and references.
- Be very deliberate about your constraints and references. I make sure every constraint, dim and reference is exactly the one I want. These are what determine how your sketch will react to model changes, a little diligence here will pay big dividends later when things change.
- Watch for Creo over constraining with the H & V constraints. It often will allow a line to be coincident with a planar surface and H or V. If that surface changes angle, the sketch fails because it can no longer be H or V.

Jun 29, 2016
10:28 AM

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Jun 29, 2016
10:28 AM

l like your idea:

- Be very deliberate about your constraints and references. I make sure every constraint, dim and reference is exactly the one I want.
**These are what determine how your sketch will react to model changes, a little diligence here will pay big dividends later when things change**. --> thats the reason why some models are only "3D picturers" that are hard to change in future.

Just to make it clear --- H & V means **H**orizontal and **V**ertical?

Jun 29, 2016
11:10 AM

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Jun 29, 2016
11:10 AM

Milan Bonka wrote:

... Just to make it clear --- H & V means

Horizontal andVertical?

Yep.

Creo likes H & V constraints, applies them liberally.