(Note: This list was prepared before the introduction of ST)
Most of us have trouble with sketches from time to time that we just canÆt get to do what we want or that keep failing. Below are some tips to help avoid this and generally improve the quality of models. Some of these arenÆt appropriate all the time but by and large theyÆll stand you in good stead. Many of these tips will apply to other CAD Software, not just Solid Edge.
1. Understand your design intent and model accordingly. This means your dimension scheme & constraints/relationships in the model should be driven by part function and match the dimension scheme of your drawing as much as possible.
2. K.I.S.S (Keep It Simple Stupid)
+ Use simple forms (rectangles, triangles, circles) if possible.
+ Use several small steps instead of 1 large, donÆt put too much into one sketch. Rather have more part features.
3. Make sure sketches are fully defined/constrained. To help this use 2 simple things which may not be turned on automatically:
+ Sketch Relationship Colors, on Inspect pull down, so you can see when you've fully constrained a profile.
+ 'Indicate under-constrained profiles in the edge bar', under tools/options/General.
4. Depending on the design intent, always try to dimension to the X, Y and Z reference planes, they never change. Try to align these to the part faces that will be datumÆs on the drawings where this matches design intent. If not to a plane then try to dimension to a face or line rather than to an endpoint.
5. Favor constraints over dimensions when this matches design intent, use construction geometry to help with this.
6. Open sketches should be used when appropriate as they offer advantages over closed sketches in certain areas.
7. Learn to use IntelliSketch, in sketch mode tools/IntelliSketch. As a model gets busier and there is more geometry to make relationships to, it may be necessary to temporarily suspend IntelliSketch, using the Alt key, or to turn some relationships off to make sketching easier.
8. Play with your sketch to see how it behaves before going to the next step, for example try changing a dimension and make sure the rest of the sketch adjusts correctly.
9. When creating patterns, it is usually better to pattern a feature rather than pattern a sketch entity. So sketch one instance of the pattern, resolve/finish it and then pattern the feature.
Not directly related to sketches but things that can have a significant impact on sketching/modeling in general.
10. Use æpick & placeÆ features such as chamfers & holes instead of sketched features when possible. For instance don't use fillets or chamfers within the sketch, unless you have a constraint that requires the clearance, add them as separate features later.
11. Try to model it like you will build it. For machining, that means start out with a large block and remove material from there. Your sketch profiles should resemble your cutting path. Molded, forged, and cast parts are not as straight forward, but the same methodologies apply. To help with this try using the feature sequence like it's ordered on the feature toolbar. So first all protrusion, then all cutouts, then all the holes and then rounds / chamfers.
There are a lot of other keyboard shortcuts that can help with sketching, for instance using A & L to switch between Arc & Line without going back to the tool bar.
Also look at the æStatus BarÆ, by default below the top ribbon bar, for tips on each operation/function.
(This FAQ was prepared with the assistance of other Forum members thread562-208631)
