Migrating from SolidWorks/Inventor I have realized that the whole sketch likes to be extruded....rather than the user selecting specific entities from the sketch. Is there any way to select certain entities to extrude so I can keep the number of sketches down?
Ex: I drew a sketch with five circles. Two of them must be cut into a previous extrusion, the other 3 must be different heights.
Solved! Go to Solution.
You can not extrude a part of sketch.
But you can directly go to extrude option at the same datum plane and go for Use(in pro-e) or project(in creo)
option and select part of sketch
The mantra for producing robust Pro/E models is "many simple features". One guideline I've heard is that a sketch should have no more than about six dimensions (although that's not hard-and-fast).
If three circles should be extruded to different heights, then use three features. (Or, possibly, use one feature and pattern-table it).
There's also no shame in referencing geometry (surfaces, for preference) created by a previous feature in order to create your next one.
If you only want one sketch to drive your whole model like it is a skeleton model then use the sketch as first standalone feature and then project the desired entities into sketches of additional features as K.Mahanta has pointed out.
Pro/E is different and IMO BETTER because there are 2 ways to create a sketch to extrude/revolve/sweep. What I suggest is this: If you do top-down design, as I do, you can create a stand-alone sketch that drives multiple parts/assemblies, and then CREATE an INTERNAL sketch that uses (use edge, offset edge) whatever elements you want from that sketch. If you're just creating a part, and if you're not going to use a sketch to drive multiple features, then the best way to do it is the Pro/E way and create an internal sketch so it doesn't clutter up your model tree like it does in S/W. There is no need to have a stand-alone sketch in your model tree unless you're using it elsewhere. This limitation is one of the things I did not like about S/W, the problem you describe. For the vast majority of cases, create ALL your sketches internal to your feature.
If I understand you correctly, you can make a stand alone sketch, and then reference it in other sketches that are internal to a drawing. From my experience, sketches can be internal in SW also and only clutter the tree the same amount that a internal sketch in Pro clutters the tree. The nice thing about extruding portions of a sketch as shown above is that you can keep it simple with rectangles, circles and squares and such verses having to get all the tangencies, alignements, perpendicularities and other relations correct in one closed loop.
One thing I know Frank is alluding to... several revisions ago, PTC started teaching users to make all sketches external to their features. This is a more SW-like approach (or was at the time). Veteran users universally hated this change. New users coming out of training would have huge model trees associated with their parts by following this method. What a mess. The supposed benefit is that you can "swap out" one external sketch for another and instantly change your feature. For example, you could swap out the sketch of a circle for a sketch of a rectangle in an extrude feature and voila, the model updates!
What they didn't bother to tell you is that half your references go out the window and your downstream features can easily fail. But then that problem was supposedly mitigated by intent chains and intent surfaces. Of course it's 2012 and probably 80% of the users still have no idea what those are even though they've been around for about 10 years now.
Overall, the external sketch debacle was really annoying to veteran users... so we prefer not to use them. Perhaps in the meantime SW has given users the option of having an internal sketch. If so... we can easily claim that they've copied us for a change! That'll fix 'em!
What Frank is saying is... you can make one 'master sketch' that handles all the relationships between geometry and then use bits and pieces of that sketch internal to downstream features as necessary. In this way, one sketch controls everything (or at least the things of primary importance). Internal sketches can pull references from the master... or they could contain additional geometry that is better left out of the master.
We need a picture... I sense that I'm not making this clear enough.
Going a little off-topic here... but there's another bug/feature with external sketches that pushed us back to internal almost immediately.
Most of our components are revolved (shafts and gears). If you use an internal sketch, you can cut any cross section through a revolved part and show the dimensions... if you use an external sketch, you can only show dimensions in the plane they were created.