Splines in sketches and the effect on checkmate

[SiW979]

Hello everyone.

We are currently in the process of rolling out checkmate in a series of phases to try and enforce our company standards and improve the quality of our modelling.

One of the Out-Of-The-Box checks we have implemented, checks that all sketches are fully constrained which as you might agree, is basic good modelling practice, it is also one of the areas where a lot of our designers tend to not do very well so the check is working well in ensuring that they adress the issue.

However! our transmissions division model lots of gears, the profiles of which are sketches which contain involute splines which are created from a template file and then the curves/splines are added to the sketch.

But, the problem now is we end up with sketches that are massively unconstrained (300+ missing) and constaining them would be a huge exercise without any benefit. On the other hand if we leave the gear profile as non-parametric or dumb curves, then it fails another check mate check which reports all swept features that have been created using dumb curves, so rock and a hard place springs to mind.

Therefore the only option I can see at the moment is to modify the check to ignore sketches in any part that is classified in TcEng as a gear?

May be one of you might be able to give me another idea as to how we can handle sketches of gear teeth.

http://screencast.com/t/M2RmN2FjMjMt

Another thing, I though the idea of studio splines was to be very easy to tweak by moving the poles around, so why on earth would you want to constrain them in a sketch anyway??????

Cheers!


Best regards

Simon NX4.0.4.2 MP10 - TCEng 9.1.3.6.c - (NX6.0.3.6 MP2 native)

http://www.jcb.com

Life shouldn't be measured by the number of breaths you take, but by the number of times when it's taken away...

 

[hudson888]

Ouch!

See while I agree that having sketches fully constrained has some merit I would NEVER insist upon it. I think doing so is probably just a bad idea for all sorts of reasons, but mainly because as you've obviously found it creates a rod for your own back. The difference between good practice in a culture of professionalism and something that a computer can police for you in place of human judgement is as large as it is generally unavoidable if you want to maintain any real efficiency.

As for the gear teeth I have a model of a gear that somebody posted here as I recall which constructs the involute as a law curve. It is as a result somewhat parametric. Where else are you getting those tooth profiles from? They look to be no better than curve data anyway and so could equally well be created outside of the sketcher. Maybe I misunderstand your process?

While we're on the subject anyone with a good parametric version on an internal metric gear please by all means post a copy


Best Regards

Hudson

www.jamb.com.au

Nil Desperandum illegitimi non carborundum

 

[JonSelby]

In the sketch you could select all lines then Insert -> Constraint
Then pick the "Fully Fixed" option which looks like three earth/ground symbols.
It would mean everything is 'constrained in space' rather than 'constrained to a feature'. It wouldn't be very nice to edit but then I can't imagine that is a particular requirement here.

Alternatively ...
If you cut just one tooth and then do a circular "Pattern Face" would that fit your work-flow?
That way you would only have to constrain one tooth.

Or have I missed the point?
I'm assuming your gear profile has some unique design characteristics and holding the formula in an Excel spreadsheet allows you to pick the diameter and number of teeth etc and spits out an 'array' of points.

 

[SiW979]

Hmmm

Hudson

When we decided that all constraints should be solved in a sketch, we were aiming it base sketches for extrudes and revolves etc as in our experience, if a sketch is left with missing constraints there is a danger of something getting moved by accident. I liken it to pitching a tent, if you decide to not secure all the guide ropes with tent pegs then expect it to wobble and be unsteady.

jonselby

Our group CAD standards stipulate that sketches must contain no more than one fixed constraint, this is to stop people being lazy and doing just as you described, this would be like emptying the tent and poles on to the floor in a heap without errecting it, but dumping a pile of rocks on top of it for our normal CAD models. Sure it won't blow away, but it's about as much use as an cigarette ash tray on a motorbike. What we want is well constructed,well thought out, fully constrained sketches that are easily edited.

However having said that, I think your idea will work for our gear profiles as the profile is never edited in the sketch, it would be recreated from scratch using our little template, therfore, there is no reason that all the curves in the sketch could be fully fixed, I would just need to tweak the checker code to inore multi-fixed constraints for that class of component.


Food for thought, thanks


Best regards

Simon NX4.0.4.2 MP10 - TCEng 9.1.3.6.c - (NX6.0.3.6 MP2 native)

http://www.jcb.com

Life shouldn't be measured by the number of breaths you take, but by the number of times when it's taken away...

 

[JonSelby]

I like your generic principle of only using one fixed constraint per sketch!
In actual fact I would go so far as to say (tentatively (so as not to upset anyone)) you should try not to use them at all.
My opinion is that its better to constrain a sketch to a coordinate system (or plane or datum), which can then be used to 'drive' that feature.
Clearly that's not appropriate in this instance.

That said ... the tools are placed there for us to use and if it fits your design culture and everyone is 'on-board' with your workflow then who's to say it ain't right (apart from JohnRBaker that is )!

 

[SiW979]

Jon

Now it gets a little deeper with our reasoning here, normally I would say exactly the same as you and certainly where a sketch is used as a base feature, I would fully contrain the sketch including locking it's position witin the sketch to a datum axis or two or plane etc without using a single fix constraint.

However if we a re using a sketch as for example the basis for a feature later in the model, and we want to copy and paste sketch around the model so we can use it for multiple similar features, then I would not position the sketch inside itself like you said, this is the time I would use 1 single fix constraint to solve the last 2 constraints, the 2 which stop it moving around in the XY plane. Then I would use external positioning dimensions to locate the sketch to the underlying model, this makes it much easier to copy and paste the sketch as there only town references which need solving. ;-)

Best regards

Simon NX4.0.4.2 MP10 - TCEng 9.1.3.6.c - (NX6.0.3.6 MP2 native)

http://www.jcb.com

Life shouldn't be measured by the number of breaths you take, but by the number of times when it's taken away...

 

[hudson888]

Simon,

Don't disagree with your intent. I just wouldn't insist on enforcing it by using checkmate when naming and shaming would do perfectly well enough as an when appropriate!

The problem as I see it would be that there are a number of occasions where it is probably going to be counter productive.

Best Regards

Hudson

www.jamb.com.au

Nil Desperandum illegitimi non carborundum

 

[SiW979]

Hudson

The problem is, we have over 300 users in 18 divisions spread 3 continents so check-mate is our way of naming and shaming, we publish league tables which got to the engineering directors and all CAD users as a way of naming and shaming.

Best regards

Simon NX4.0.4.2 MP10 - TCEng 9.1.3.6.c - (NX6.0.3.6 MP2 native)

http://www.jcb.com

Life shouldn't be measured by the number of breaths you take, but by the number of times when it's taken away...

 

[hudson888]

Okay Simon,

Here's the rub. NX is a powerful and flexible tool which regularly offers multiple solutions to any given problem. You may theoretically be able to police the sketches but there are a range of other things that you and I both know that neither your nor I nor anyone for that matter can police. We also know that within that framework there are several far more important things that go towards differentiating quality models from something that exists within a state of anarchy. Good modelling practices need to be culturally instituted within any organisation. I'm presuming that any organisation such as your own which depends on good design for its success that such a culture of professionalism already exists. If it exists (as I believe it has to), then mine would be the decision to allow latitude rather than including that check with checkmate.

Or in other words some of your users are liable to opine that this level of control being imposed isn't really all that useful or necessary. Its advice that you asked for so mine is that the term "best practices" is all too frequently interchangeable with "lowest common denominator". I'm a CAD designer. I don't really like being called a draughtsman. I solve problems by thinking creatively. I would never even dream of modelling the same thing twice using the same method, because I can always think of a better way. If you want creative people to do remarkable things to move your company forward then wherever possible a lighter hand on the rudder will produce better results.

Best Regards

Hudson

www.jamb.com.au

Nil Desperandum illegitimi non carborundum

 

[JonSelby]

Simon,

Your use of copying and pasting sketches is interesting, and yes I can see that a local ground would be useful.
I would presume you are happy to lose associativity between the various copied-n'-pasted sketches.
I've only every copied sketches to other models in which case any references, external to the sketch, are recreated within the paste process.

As far as "naming and shaming" goes I think a little inter-team rivalry is quite healthy.
And as I always say "a blame culture is better than a lame culture"

 

[SiW979]

Hudson

As ever your clarity and reasoning is logical, however we are very differnt to the way you work, sure we have CAD models which are only modelled once, but the vast majority of our parts are used over and over again, we have parts that have been saved as many times, and we encourage reuse of data where ever possible, our engineers also move from division to division so it makes sense if they are plug and play engineers, who can make the transition seamlessley between business units.

To ensure this happens, we have lots of standards in place to make sure that everyone works to the same level. Also we need to ensure that is designer A who has 20 years experience using CAD creates a model and suddenly goes on gardening leave because he is joining CATERPILLAR (spits on floor)and this happens regularly as they are only 35 miles away, that whoever picks up there part can get to grips and understand the way it has been modelled so they can pick up where they left off.

If everyone had the level of understanding of you and I, then this wouldn't be so much of a problem, but we have all differnt levels of experience here, so while I love trying new processes, and developing new methods (to JCB anyway) and demonstrating them to our CADET (CAD Evolution Team) in theory, there will be many people who would stuggle to understand some of the processes and concepts. On top of this a lot, in fact the vast majority of our work is not ground breaking innovative parts, they are just brackets, plates and WA's that hold on all the hi-tech systems we procure from specialist companies who deal in the hydraulic and electrical systems we use and it is these parts where we want to ensure are all modelled using the same principals and processes.

As I said, I can see your point, but what I'm aiming at is what I term good house keeping, black and white stuff like naming sketches something other than SKETCH_000, ensuring that people do not position holes centerd to blends, that only 1 primitive is used per model. Because what we have found is that people tend to be very very lazy when it comes to doing the most basic of tasks correctly.

Best regards

Simon NX4.0.4.2 MP10 - TCEng 9.1.3.6.c - (NX6.0.3.6 MP2 native)

http://www.jcb.com

Life shouldn't be measured by the number of breaths you take, but by the number of times when it's taken away...

 

[SiW979]

Jon

We don't loose any associativity, infact, when you past the sketch, you get the option to create a brand new sketch which will get a whole new set of parameters so it can be controlled and sized independantly to the original, it can be created as an instance of the orgiginal in which case the original sketch drives the size of the new sketch, or as a link to the original, in which case expressions will drive both ways.

I agree with your statement regarding a little competition being healthy, we have seen a dramatic improvement in the 6 months since we started rolling out the checkmate, also it has made a lost of the old times (who dont't like change and think sketch is a black art and an implement of the devil) address sever long time skills gaps which they have managed to hide for all these years. The amount of parts that good CAD users pick up and think "aha! a quick save as and tweak to the sketch profile etc and I'll have saved myself a few hours work" only to find out that the model was created using exctracted and dumb curves.

Best regards

Simon NX4.0.4.2 MP10 - TCEng 9.1.3.6.c - (NX6.0.3.6 MP2 native)

http://www.jcb.com

Life shouldn't be measured by the number of breaths you take, but by the number of times when it's taken away...