Advantages of a fully defined sketch

Anonymous

Advantages of a fully defined sketch

Anonymous
Not applicable

Hello there!
I have been working with Inventor a couple of years but I still learn about Inventor. In this opportunity I would like some support by naming the advantages of fully defined sketches.
I always define each geometry in a sketch so in the end the sketch is fully defined and has blue colour. However, I was asked recently about the reason to fully define sketches and I just could think on two valid reasons. 

  • The complete part is in the end more stable and reliable.
  • Fully defined sketches are a key to model an iPart due to desired relationships between parameters.

 So if you can add oder reasons or correct me, please do so and enlighten me!

Regards,

Andres 

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Curtis_Waguespack
Consultant
Consultant

Hi andresgd.1,

 

Once a sketch is fully constrained, the sketch "solver" is happy and isn't trying to "do stuff", so fully constraining can help with performance. 

 

Also if the user is keeping things simple, fully constraining a sketch is never an issue:

http://inventortrenches.blogspot.com/2011/03/inventor-101-simple-fully-constrained.html

 

I hope this helps.
Best of luck to you in all of your Inventor pursuits,
Curtis
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Cadmanto
Mentor
Mentor

To piggy back what Curtis said, a fully defined sketch prevents the unexpected.  If you have ever noticed while defining your sketch, and changing values, sometimes in the process your sketch will change to something not only undesirable, but just plan whacky.  So, if you don't fully define it, and you change it in the future, it can go ari.  The only time I don't fully define a sketch is when I have splines or irregular shapes.

 

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PaulMunford
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Fully constrained = Fully predictible ๐Ÿ™‚

 


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JDMather
Consultant
Consultant

@Anonymous wrote:

..... valid reasons. 

  • The complete part is in the end more stable and reliable.

I would think that is reason enough.

 

But if you need another reason - to pass my class, you must fully define your sketches, or I will see you in class again next year if you elect to not change majors.  Smiley Surprised


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johnsonshiue
Community Manager
Community Manager

Hi! When the part or its features are still being modeled, keeping sketches under-constrained may help you make changes more quickly. However, when it is approaching complete, you will want to fully constrain the sketch. It is because you don't know if the sketch has been changed inadvertently or mistakenly violating the design intent.

The point to create a sketch is to define a rigid shape (solid or surface). If a sketch isn't fully constrained, it is like designing a flexible part.

Many thanks!

 



Johnson Shiue (johnson.shiue@autodesk.com)
Software Test Engineer

YannickEnrico
Advisor
Advisor

I second what almost everyone said.

 

You get a more stable part by having it fully constrained.

 

As I understand from what someone once told me, constraints are better than dimensions - And even if dimensions are correct when placed, you should always delete trailing zeros. 

 

You know what to expect when changing something, because your geometry is not "floating". 


The disadvantage to this, being when you change your geometry so it has less corners than before - Because then you'll miss some projected geometry. 

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Anonymous
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If you are around as long as I am you would know that "old" software forced you to have fully defined sketches. I don't think any of those are still around. The key to this however still exists : computers work with data and all data is defined. In the case of sketches, even a loose line has coordinates for start and endpoint.

 

One aspect of "fully defined" has been mentioned a lot in this post : defined geometry reacts predictable.

 

A second aspect was less exposed : defining a sketch forces you - the operator - to think about design intent. Do you want a line to be vertical, perpendicular to another one, parallel or colinear ? It may be the same line in your sketch but it behaves differently. Is it important that your sketch stays aligned to a major axis in the part or should it stay at a distance from an edge ?  Should a cutout stay "open" on the edge of your part or can it turn into a hole when the part grows in size ?  These are only a few examples of what you should be thinking about when designing and sketching.

 

A good way to do this is unfortunately not what most handbooks and help functions point you to. It is sketching without constraints, in Inventor by keeping CTRL-key pressed. After the loose sketch you make it behave as intended by applying dimensions and constraints. Advantages : you are sure about dimensions because you explicitely enter the numbers and you are sure about the relations and constraints. Further advantage : you see the sketch modifying as you go along. Disadvantage : Inventor can make strange moves, depending on the order in which you proceed, so some caution and experience is needed.

 

Working as above also enforces simple sketches. It's hard to make intelligent relationships when you exceed 10 to 20 elements. Which is a good thing to keep your design healthy. Consider it sculpting. Start with the big block and add details as you go along.

 

My 0,02โ‚ฌ

swalton
Mentor
Mentor

Expanding on @Anonymous post...

 

I tend to make my sketch dimensions match how I plan to dimension the feature on my drawing views as well as how I expect the component to change through its life from prototype to obsolete part.  It makes me think about how the machinist will create that feature, how it might be inspected, and how it will fit with the other components in my design. I add the tolerances to the sketch dimensions as soon as I know what they need to be.  That way when I wait 2-3 months between the design of a bearing journal and documenting it on a print, I don't forget the correct values. 

 

I find that if I take the time to think about those 2nd and 3rd steps in manufacturing my design, I get a better result.  

 

A key thing to remember is that the original designer may not be the one to make a revision to the model.  If the sketches are not fully defined it can be hard to understand all the downstream effects of changing a dimension value. 

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mcgyvr
Consultant
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@Curtis_Waguespack wrote:

Hi andresgd.1,

 

Once a sketch is fully constrained, the sketch "solver" is happy and isn't trying to "do stuff", so fully constraining can help with performance. 

 

 


This..

I have seen many issues further down the line where the fix was to simply fully define the sketch.. The fact that it had needed dimensions/constraints caused the solver to "make the wrong choice".. It will solve.. But there could be multiple solutions.. Don't let it choose for you.  

 

Fully defining a sketch is the right way.. Plain and simple... 

Don't do that and you are guaranteed to cause yourself or someone/something else to "ass-u-me" 



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Anonymous
Not applicable

I agree with the comments 100%...  I understand whats being said completely but how do you explain it in the simplest form to someone with no capacity to accept fact?  We have a perfect example of a sketched symbol in an idw template that turns pink, (unable to solve) as soon as you touch it.  His workaround is to keep trying and deleting dimensions until it will let him freehand the edits he wants to make.

 

Basically is there a way to quantify in terms of time, both computer processing and user input, what this bad practice is costing?

YannickEnrico
Advisor
Advisor

@Anonymous wrote:

 

Basically is there a way to quantify in terms of time, both computer processing and user input, what this bad practice is costing?


With someone who won't listen to reason, I'd just ask them to find a clock, and start the timer every time they do something like this.

And then ask them to properly do the sketches - And measure how long it takes to make similar edits, then.

 

 

I'm not sure if there is a tracker, or if the difference is big enough in just a simple sketch, to look at the resources it uses - but it might be worth a try. 

If it's an assembly with a lot of parts, you may see a difference?

 

 

 

Also... do you ever produce something that is wrong? Based on the 3D? Is it wrong because of this bad practice? I guess you could always argue that there wasn't spent enough time on it, but with proper sketch practice, you'll need to use less time on it to make it correct any way? See above. 

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Anonymous
Not applicable

Stephen,

 

One of the problems with the geometry solver is that it doesn't warn you for possible over-constraining. Take a triangle with a 90ยฐ angle where you put "5" on one of the short sides, "5" on the other short side and then 45ยฐ on the sharp angle. No protest. Change one of the "5"s into something else and you're stuck. In this case it is easy to see why it doesn't work. Make the sketch with 50 elements and you don't have a clue anymore. So rule 1 : keep sketches simple.

 

Something else is the automatic constraining in IV. Sorry to say so but it sucks. If you are freely sketching it will constrain everything to anything else. Even dragging elements will activate automatic relations, creating unwanted connections behind your back. My rule 2 : except for endpoint connecting I will add intelligence to my sketches myself. No software can read the design intent from my eyes.

 

A well designed part with well organised sketches and relations will stand a dimension change in step 5, leaving the next 25 steps behaving in an orderly manner.

 

Alex

kpyoung333
Enthusiast
Enthusiast

I used to design doors and made templates using the "muscular modeling" technique where you derive parts that will update easily. The issue with unconstrained - or more importantly incorrectly constrained - parts is that when you change the dimensions with iLogic Forms things go nuts. The most obvious would be when changing the vertical dimension first, the door arch would bow outward instead of staying less than 90ยฐ like a real door arch would. If the dimension was lowered again the unconstrained line would always want to stay bowed out and never go back inside like a normal door arch. Would have to reopen the template and make sure the dimensions were adjusted by width first then height. Eventually I went back to redo the sketch, which had many projected lines that then broke. If you set things up properly from the beginning you won't run into monumental unforeseen headaches in the future. https://youtu.be/MXZ5b98WiiA

johnsonshiue
Community Manager
Community Manager

Hi Stephen,

 

The sketch symbol behavior sounds like a bug to me. Could you post the example or send it to me directly (johnson.shiue@autodesk.com)?

Many thanks!

 



Johnson Shiue (johnson.shiue@autodesk.com)
Software Test Engineer
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