that sketch will become too complicated,difficult to manage and slow down the computer.
Easier method to simply make a single feature and pattern.
Making sketch simple comes under best practices.
Would not recommend using the pattern tool within Solidworks sketch also..simply because making a fully defined sketch as i want will be time consuming.
You can join PTC technical committee for modelling to give your recommendation.
As a work-around you could pattern the sketch feature. After that you could create another sketch referencing the patterned sketches.
I use sketches as calculators...
Yes they can be very complex but not for the obvious reasons.
This sketch is very hard to sustain , but it is exactly what it needs to be.
(stellar dodecahedron with the center at the origin and a specific size)
his one sketch governs the entire design with one dimension.
The other two dimensions help is visually manageable.
I wouldn't do it any other way.
I often use streamlined "skeleton" sketches that I then reference in a final sketch. This allows me to lock down and simplify the most important relations and then the more intricate details of the final sketch are kept separate. as a simple example, you might have a complex polygon that you want to have radii on. it is much easier to sketch the radii-less polygon and then in a subsequent sketch use edge, pick the loop - and add a bunch of fillets to the sketch.
you might think, well why not keep it simple and in one sketch? actually it's not as simple to have in one sketch. if it fails - you can see where it fails. and for my example, the dragging the radius bigger or smaller doesn't affect the shape of the polygon, etc.
when I need a sketch to have a pattern, I often will create the prototype shape, then pattern it, then create the final sketch and just use edge -> loop.
if you don't like to see separate sketches, then group them.
it works, it works well, and it's just the way this software works. I personally wouldn't mind if there was a way to create patterned sketch features within a sketch. however it would just be a novelty to me. after 20+ years using pro|E / Creo, I can confirm - simple sketches are more robust. and more complex sketches are more robust when broken up into multiple steps.
The attached video shows this 2-sketch method. it's for a complex polygon and a simple radius. if you included the radius in the original sketch dragging would be horribly unwieldy. Anyway - the same concept works for patterns.
So to sum up I conclude that if we pattern in sketch mode
1) Sketch will be unstable and there will be no associativity or connection between sketch pattern members like in feature pattern
2) It will be very difficult to increase the no. of pattern, angle or spacing members after sketch pattern as there are no connection between pattern members.
But for information, I would like to say that in Autocad 2013 to 2017 Autodesk have introduced a property called array associativity. If you select the members after array the array will be selected as a group. You can also explode it and make separate anytime you want. Though I am aware that autocad is primarily a 2d drafting software and nothing comparable to feature-based, parametric 3D CAD software like PTC Creo but if this feature can be applied in creo sketch then one can easily get a feature pattern like sketch-pattern.
What do you think?
I am interested to know what other Creo users think about this.
What about fully defining the complex sketch?How will creo define how to dimension it?
Anyways if you have current maintenance for Creo you can put up this in PRODUCT IDEA.
from my point of view, discussions similar to this one are "academic", only (unfortunately). I think it is better to accept current functionality of software (not only Creo), if someone use it to earn someone's living. I agree with you that any software can be improved, but it is not possible to fulfil every user wish .
Your summation is correct for SolidWorks, yes. Since the feature doesn't exist in Creo, there can be no conclusion other that the fact that if PTC were to build the code for this feature, it wouldn't have those limitations. Maybe a few bugs, but you will find that PTC does a much better job of defining new functionality than SolidWorks. SolidWorks was created in large part by users' -demands- and therefore you have some half baked solutions. In SolidWorks, try patterning your first extrude in the sketch where it creates more than one solid... it can't. Exactly where you would like use it. Sketch patterned features must be a single closed sketch or it has to merge with something if it creates multiple solids. How dumb is that!
You can always copy paste the entities you want and then, select the first one and the copied one copy it again and paste it ad infinitum while changing the offset in the required direction. But, as pointed out in the other answers, it will complicate your sketch.