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How do I know my sketch is definitive ?

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How do I know my sketch is definitive ?

Hi All

I use Creo 2

since choosing which dimensions  could be  strong and which ones weak is completely manual in Creo, untill it goes to conflict. I would like to know, if there is anyway to understand that my sketch is definitive ( like in solidworks) , cause I am used to that, and I complete the sketch to the point that all the lines are black and can not be modified by dragging them around

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Re: How do I know my sketch is definitive ?

Let's instead use Ron's image from below:

bluedim.jpg

All weak dims.

Let's say I change the 202.331 dim to be 300.000.  This is what will happen:

  • The left end is constrained to the reference and therefore won't move.  So, the right hand vertical line will move to the right.
  • The vertical line below it is tied to it so it will move right too.
  • The length of that second vertical line is fixed (114.836) so it will not change.
  • That will drag the bottom angled line to the right as well.  It will not change angles because it is constrained as normal to the leftmost angled line.
  • Because the bottom most horizontal line has a fixed length (74.649), it and the short vertical line at the left will move right as well.
  • The far left bottom point is constrained to the reference and will not move.

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.

--
Doug Schaefer | Experienced Mechanical Design Engineer
LinkedIn

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50 REPLIES 50

Re: How do I know my sketch is definitive ?

One rule that helps most user is to never leave weak dimensions. Those are "arbitrary" dimensions that creo adds to keep the sketch fully constrained. The rarely correspond to design intent.

There is one more dimension option in sketcher, LOCK. If you lock a dimension, it can not be changed by dragging.


Steve Williams
Pro/E Version 15/16 (Circa 1995/1996)

Re: How do I know my sketch is definitive ?

I suggest you set the color scheme such that weak dimensions and constraints are shown in bright red.  Your goal is to eliminate the red!

I use this config.pro setting:

sketcher_dimension_autolock yes

This means that whenever I type in a value for a dimension, it will become locked (so it can't be changed by dragging the geometry around).

If I am in the concept phase, I unlock some dimensions so that geometry can be dragged around in the 3d model, but my ultimate goal is to have all dimensions locked.

Re: How do I know my sketch is definitive ?

In SW, a sketch can be made and not constrained at all. All the sketch entities will be blue and there will be no dimensions, yet you can complete the sketch.  (How SW updates those sketches, I have no idea.)

In Creo, all sketches are fully constrained (what I believe that you mean by "definitive") at all times.  There's no such thing as an under-defined sketch (what would be a "blue" sketch in SW) in Creo.

Initially, however, all the dimensions and constraints (equal length, horizontal, vertical, tangent, etc) are placed by the software.  Those will be gray in color so you know that they aren't your contraints & dims, they are Creo's.  So, although the sketch is automatically fully constrained, as has been said, it isn't likely constrained as you want it.

--
Doug Schaefer | Experienced Mechanical Design Engineer
LinkedIn

Re: How do I know my sketch is definitive ?

I've an angle about this: SW company took the time to implement ideas that enhance the user experience.

In its sketcher, SW doesn't bother the user with what weak dimensions and constraints it imposed on the geometry behind the scenes in order to "solve the sketch".

It instead gives the user the pertinent information by color coding the geometry that the user has "locked down" (black) and what can still be manipulated (blue).

Creo already has all the building blocks to make its sketcher behave in the same manner - but they don't do it, maybe because of IP issues.

Re: How do I know my sketch is definitive ?

Or because it's a terrible idea.

I agree on the SW philosophy of making things simple and not giving the user info they don't think they need.  But, I need to know how you are constraining my geometry.  I hope Creo never implements anything like this. One of Creo's strength is the amount of info it gives you on the status and structure of your model.

Best I can tell, SW simply leaves the unconstrained sketch entities at the same location relative to the part origin as the model changes.  But there's no real way to know, because SW doesn't tell you, and therefore no way to predict how your model will act.

--
Doug Schaefer | Experienced Mechanical Design Engineer
LinkedIn

Re: How do I know my sketch is definitive ?

??? I don't think it's a terrible idea.  I maintain that Creo could steal a lot of good ideas from the Solidworks sketcher.

You can predict exactly how a model will behave in SW if you make sketches that are fully constrained.

Or you can leave the sketches blue (these are basically full of weak dimensions - you just don't see them)

In fact, in SW there is an option to prohibit the creation of "blue" sketches.

If I remember correctly (it's been few years), there is a ton of useful tools that will guide you about what in your sketch is constrained, unconstrained, external reference, overdefined, etc...  So it's quite easy to make a fully constrained and well behaved sketch.  Then there patterns, ease of making and editing splines and polylines, and useful constraints such as "pierce" - all things that are missing from the Creo sketcher.

Anyway, I digress; this was about constrained vs. unconstrained sketches.

And I think it's a complete illusion that Creo is better because it does not permit unconstrained sketches and Solidworks does.

Suppose that a user made a Creo model based on a sketch comprised entirely of weak dimensions and constraints.

Can you really predict how such a model will behave if you change one of the dimensions?

Re: How do I know my sketch is definitive ?

My comments were on unconstrained sketches.  You have no information on how SW handles those.  I find no value in an unconstrained sketch in a parametric modeler, only uncertainty.  That's what I was calling a terrible idea (somewhat, but not entirely, tongue-in-cheek ) and one that I hope never finds a home in Creo.

As far as being able to predict how a Creo sketch made only with weak dims & constraints will behave, I can absolutely do that because I know that it's going to maintain this distance, these things horisontal, these things equal, etc. all relative to the references selected.

I didn't intend to open a SW vs. Creo debate, there are way too many of those already.  I merely wanted to point out that all Creo sketches are fully defined by default, there's no such thing as an unconstrained sketch, like there is in SW.

--
Doug Schaefer | Experienced Mechanical Design Engineer
LinkedIn

Re: How do I know my sketch is definitive ?

Ok, we can agree to disagree about that terrible idea.

And as far as being able to predict how a weakly-constrained creo sketch will behave - this is what I had in mind when I asked the question:

bad_sketch.png

Fully parametric; but can you really predict what will happen if this dimension is changed to be 40?

Re: How do I know my sketch is definitive ?

You can turn the display of weak dimensions off so only strong dimensions (ones you define show) in the sketch. There are also entity locks that you can place and show. Entity locks can be place by selecting the entity, RMB, and select Lock. RMB in the graphics area of the sketch and you should see Show Entity Locks or Hide Entity Locks depending on current settings. You can also set it by selecting an entity and Toggle Lock under the Operations section of the Sketch tab. If Show Entity Locks is turned off when your cursor hovers over a locked entity a pad lock looking icon displays.