Let's instead use Ron's image from below:
All weak dims.
Let's say I change the 202.331 dim to be 300.000. This is what will happen:
I also know that if that vertical reference moves right or left, this entire sketch will move with it because there are no other vertical references.
Now, if I grab a line and drag it, Creo will allow the values of the weak dims to change. It also allows the values of string, non-locked dims to change, I believe, so no difference there.
All predictable because Creo tells me what till happen. Now the default scheme here creates a lot of cascading effects, but it's fully constrained and predictable.
If we sketched the same thing in SW all the lines would be lue and there would be no dims or constraints. I could grab and drag any line pretty freely and usually, only that line moves. What isn't clear, however, is what happens to the sketch if the rest of the part moves.
You mentioned below that Creo's weak dims and SW's blue sketches are the same. The above is why I say they are not. My point was not to critique SW (which I guess I did), but to answer the original question. The two sketchers do not behave the same, there are differences in methods that are important to understand if you are coming from one and want to bake robust designs in the other. There isn't really an equivalent of the "blue sketches" of SW, but I guess the image above is as close as it gets. It still provides a lot of info on how this sketch will behave, the default SW sketch provides almost nothing. Different ways of doing it and I strongly prefer Creo's.
In either tool you need to master it and put in the right inputs to get good results. Each tool, however, requires different inputs to get there.
I don't have access to Solidworks anymore, but signed up for free trial of Onshape; I'm pretty sure it uses similar technology (it's the same team, after all).
So far as sketcher is concerned so I can at least say that these are the rules you need to know about: if it's blue, it will stay in place*, and you can drag it around. If it's black it is constrained (and you can't drag it - this is actually where Creo sketcher is superior because of the extra control you have with the dimension lock/unlock)
* blue sketch will remain fixed relative to the part origin; for example, if the underlying solid is changed,:
Probably not what you want to happen, but it is not really unpredictable.
And so I agree with you about these tools being different and the requirements of understanding the principles of robust design.
However, for me, having auto-created dimensions does not provide much benefit - I still end up dimensioning the sketch according to my intent.
So for Creo, strategy is to "eliminate the red", and for Solidworks, it is to "eliminate the blue".
Thank you for your answer. Yes there might be a blue condition until I put those same geometrical constrainst as well.
But there's one point that the sketch is totally definitive, that Creo doesn't tell me, and I have to apply one more constraint, get the error ,and understand that the sketch WAS ALREADY definitive.
My aim is to understand : is there any other way to avoid that one more move ?
not all the sketches are possible to judge and reason by looking at. after they become too complex
Keep your sketches simple is the best advice. It's okay to use multiple features.
If your sketch is too complex to judge and reason by looking at it, it's way to complicated!!
It really would be nice to have a little light that says " You have successfully constrained your sketch completely. No Creo assumptions remain."
However, to suggest SW actually has anything over on Creo in Sketcher... No Way! Life is too short for the SW sketcher if you don't do shortcuts. I don't do shortcuts.
As to capabilities of the SW sketch; some good, a lot of really tedious stuff. And the overhead on the computer is noticeable on workstation laptops. Every pick has a delay so the menu system can catch up. Tedious, I tell you! And I've done it.
If you are wanting to understand how many constraints and/or dimensions you need to fully define a sketch you'll need to know what your your geometry is, what the intent is, the constraint you are using to control the geometry, and what the constraint is controlling. The one constraint that will allow you to do what I think you are asking is the coincident constraint as it can control more than one constraint at a time which will allow you to completely define the sketch geometry but not have to specify all constraints, so you could still specify more constraints but the conflict dialog would not show. You could see this in the sketch Doug discusses above. On the left-hand side of the sketch where the 109 degree dimension is you could remove the two coincident constraints at the line end points and change it so the line is coincident to the horizontal reference line. You have one less constraint shown, the sketch is fully defined, and you could add a horizontal, parallel, or perpendicular constraint to the line and you wouldn't get the conflict dialog.
I respectfully disagree. Last time I used Solidworks for work was version 2008. Maybe they threw in too many eye-candies that in 2017 slow down even modern laptops. Nevertheless, I recall many things that were worthy of copying:
- Solidworks: pierce constraint - ability to reference geometry that is not perpendicular to the sketch plane. In Creo, you have to go about this by setting up datum planes and points ahead of sketching.
- Solidworks: splines - you could create splines that were a mix of straight and curved segments, and you had good control over every node. In Creo, splines are a bit of a non-parametric odd-ball. Wait, why can't I make this spline tangent to this other line in my model? ( Need Help with Spline Control )
- Solidworks: after you sketch out your shape and place the 1st linear dimension - the rest of the sketch is scaled to preserve the overall shape and satisfy the prescribed dimension. In Creo, you have to do the dimension modify trick to do the same thing, otherwise, it's a garbled mess. ( Sketcher scaling automatically with first dim change. )
- Solidworks: have tools that interrogate the constraints and help you eliminate the ones that overdefine your sketch, or are external to the sketch.
- Solidworks: ability to simply copy and paste a sketch within the model. Creo, you have to save it to disk and then import it after setting up a new one.
- Solidworks: internal sketch can be dragged in the model tree to be before of the boss feature and thus become an "external" sketch and the basis of other features. Creo: no such luck; you didn't think ahead, so we punish you! Back to save to disk and import workaround.
- Solidworks: blocks - reusable shapes that can be repeated throughout the sketch. Creo sketch palette is good, but it is hard to use for newcomers, and what's up with having to always reset the scale of an inserted sketch palette item?
You might scoff at all these shortcuts, but Cad software market share says otherwise...
No problem, you may disagree.
Everyone has their own needs. I've seen full suites of SW thrown out for a full Creo install just for it style capability.
But for me, I know how to draw in Creo... very well, I might add. And I cannot say that my abilities in SW, and I've tried.
I though some of Creo's detailing functions were cryptic until I saw what SW does. No, I don't have time for that.
Overall, when you add detailing requirements to my job, I am 50% faster on Creo, and that is because I understand it well, inside and out.
Therefore, I will always have a bias toward Creo... but I cannot recommend it for everyone.
When do you think you can select a perpendicular surface for your sketch reference in SW? Just teasin'
And to give credit and maybe a tip; there are some not-so-obvious features behind the Creo spline. It is a matter of learning to click just right.
For those that have a practice or requirement to not have any weak Sketch dimensions, you could consider the following mapkey, which selects all dims and converts them to Strong.
! *** mapkey for Sketch mode to select all dimensions and convert all to Strong
mapkey w2s @MAPKEY_NAMEselect and convert all dims to strong;\
mapkey(continued) @MAPKEY_LABELconvert all dims to strong;\
mapkey(continued) ~ Open `main_dlg_cur` `Sst_bar.filter_list`;\
mapkey(continued) ~ Close `main_dlg_cur` `Sst_bar.filter_list`;\
mapkey(continued) ~ Select `main_dlg_cur` `Sst_bar.filter_list` 1 `2`;\
mapkey(continued) ~ Command `ProCmdEditAll` ;~ Command `ProCmdEditWeakStrong`;;