Tips for robust sketches 12

[KENAT]

Does anyone know of any kind of document or something similar which has a list of tips or a design guide for making robust sketches?

I have at least 2 colleagues who've had trouble in this area and just keep complaining and saying things like "it's not as good as Pro E" or "it's not as user friendly as Solid Works" or "this is why it only has 3% of the market" etc.

I've tried to share what I know (although largely self taught I’ve been using SE since 1999 and like to think I’m fairly good) and we actually have some guidelines in our Design Room Manual but neither of them pay much attention.

Even if you don't have any references maybe if any of you can give your top 3 or 5 or whatever tips.

Sorry if it's a bit of a rant but I just had to walk away from one colleague before it got ugly!


KENAT, probably the least qualified checker you'll ever meet...

 

[Schipperus]

Kenat, I know exactly what you mean...

Just the other day someone asked me why his chamfer aded material instead of removing it. It turned out there was a very thin layer of material over the edge, because one profile wasn't fully constrained...

The steps I usually teach new emplyees are:

1- Use simple forms (rectangulars, triangles, circles) if possible.

2- Always constrain your sketches fully, this means no open profiles.

3- Use many small steps instead of 1 large (don't put details in the profile).

4- Try using the feature sequence like it's on the feature toolbar. So first all protrusion, then all cutouts, then all the holes and then rounds / chamfers.

IJsbrand Schipperus

 

[toffeet]

Hello Kenat,

For me the golden rule is that designers need to fully understand the intent of their design and what relations and dimensions need to be added to drive that intention. Too often I see someone just adding dimensions and relations until the sketch is fully defined. Unfortunately there is no manual for this and it boils down to the skill and the intelligence of the designer.

I do have the following tips:

1.Don’t put too much into one sketch. Rather have more part features.
2.Depending on the design intent, always try to dimension to the X, Y and Z plane. They never change.
3.Make sure sketches are fully defined.
4.Rather dimension to a face or line than to an endpoint, especially when using inter-part copies. Someone might just put a chamfer on that other part and then your endpoint will be gone while the face is still there.

Regards,
Theodore


Solid Edge V20 SP1 on WinXP SP2

 

[PatCouture]

The tips mentionned above are a very good start.

I could not agree more with toffeet on the fact that you have to fully understand your design intent!

Other guidelines I like to remind myself.

5. K.I.S.S
6. Play with your sketch to see how it behaves before going to the next step.
7. Favor constraints over dimensions when possible.

Patrick

 

[swertel]

In SolidEdge, always use open profiles where possible. I don't know if Schipperus is confusing me or not, since he mentions it in the same line as fully constrained.

Sketched should always be fully constrained so changes are predictable. But, one of the things that makes SE so powerful and unique compared to other MCAD packages is it ability to use open sketches. They are more robust than always using a closed profile because there are fewer entities to change during a modification.

8. Don't use fillets or chamfers within the sketch, unless you have a constraint that requires the clearance.

9. Model it like you will build it. For machining, that means start out with a large block and cut out material from there. Your sketch profiles should resemble your cutting path. Molded, forged, and cast parts are not as straight forward, but the same methodologies apply.

--Scott

http://wertel.eng.pro

 

[toffeet]

With regards to the 2 colleagues:

"Bad craftsman always blame there tools."

Regards,
Theodore

Solid Edge V20 SP1 on WinXP SP2

 

[KENAT]

Well thanks all, I think all the things you put are things I do. Quite a few of them are already in our DRM and are things I've tried to explain, especially the KISS associated rules.

toffeat, couldn't agree more on the bad workmen, though I suspect we all do it from time to time.

I find it interesting that they both apparently have chosen not to attend any of the more advanced training sessions we've had over the last year or two. Now, the training isn't actually that good (a separate issue) but it's almost as if they don't want to learn, they'd rather just complain that it's not Pro E/SW.

(Sorry for the rant, first & second email I opened today were from one of them stirring on this issue.)

Thanks again, really appreciate it.


KENAT, probably the least qualified checker you'll ever meet...

 

[beachcomber]

Kenat,

Put them back on the drawing board !!



bc

 

[KENAT]

Trouble is, then I'd be really out of my depth as except a couple of minor changes, I never did drawing board;-).

KENAT, probably the least qualified checker you'll ever meet...

 

[Schipperus]

Swertel, thanks, you're totally right. Open profiles are one of the kicking features in Edge. I was wrong. Open profiles are OK as long as they are fully defined too....

And PatCouture. Maybe because I'm not native English, what does K.I.S.S. stand for??? I really love computers, but I hope it's an abbreviation...?

IJsbrand Schipperus

 

[donyoung]

Keep It Simple (and) Stupid

 

[toffeet]

We once had a political party in South Africa with the name KISS (Keep it straight and simple). I think they got like 400 votes in total in a national election.

Solid Edge V20 SP1 on WinXP SP2

 

[SLemin]

I'd recommend a few simple things which may not be turned on automatically - Sketch Relationship Colours (on one of the drop down menus) so you can see when you've fully constrained a profile. and 'Indicate under-constrained profiles in the edge bar' (under the tools/options)

 

[KENAT]

Thanks Slemin, I use both those and have shown several users how to use them.

KENAT, probably the least qualified checker you'll ever meet...

 

[KENAT]

OK, I tried to put all the comments together. It's not particularly well laid out but might work. What do you all think and is it worth making into a FAQ? (I went through our DRM and almost all of them are at least implied if not explicitly stated in it.)

ROBUST SKETCHING TIPS

Most of us have trouble with sketches from time to time that we just can’t get to do what we want or that keep failing. Below are some tips to help avoid this and generally improve the quality of models. Some of these aren’t appropriate all the time but by and large they’ll stand you in good stead.

1. Understand your design intent and model accordingly. This means your dimension scheme & constraints/relationships in the model should be driven by part function and match the dimension scheme of your drawing as much as possible.

2. K.I.S.S (Keep It Simple Stupid)

Use simple forms (rectangles, triangles, circles) if possible.

Use several small steps instead of 1 large, don’t put too much into one sketch. Rather have more part features.

3. Make sure sketches are fully defined/constrained. To help this use 2 simple things which may not be turned on automatically:

Sketch Relationship Colors (on one of the drop down menus) so you can see when you've fully constrained a profile.

'Indicate under-constrained profiles in the edge bar' (under the tools/options)

4. Depending on the design intent, always try to dimension to the X, Y and Z reference planes, they never change. Try to align these to the part faces that will be datum’s on the drawings where this matches design intent. If not to a plane then try to dimension to a face or line rather than to an endpoint.

5. Favor constraints over dimensions when this matches design intent, use construction geometry to help with this.

6. Open sketches should be used when appropriate as they offer advantages over closed sketches in certain areas.

7. Learn to use intellisketch. As a model gets busier and there is more geometry to make relationships too, it may be necessary to turn some relationships off to make sketching easier.

8. Play with your sketch to see how it behaves before going to the next step, for example try changing a dimension and make sure the rest of the sketch adjusts correctly.

Not directly related to sketches but things that can have a significant impact on sketching/modeling in general.

9. Use ‘pick & place’ features such as chamfers & holes instead of sketched features when possible. For instance don't use fillets or chamfers within the sketch, unless you have a constraint that requires the clearance, add them as separate features later.

10. Try to model it like you will build it. For machining, that means start out with a large block and remove material from there. Your sketch profiles should resemble your cutting path. Molded, forged, and cast parts are not as straight forward, but the same methodologies apply. To help with this try using the feature sequence like it's ordered on the feature toolbar. So first all protrusion, then all cutouts, then all the holes and then rounds / chamfers.


KENAT, probably the least qualified checker you'll ever meet...

 

[beachcomber]

Hi Kenat,
That's a great list, and should be pinned on the wall next to every user.
I would think the list would apply to almost ANY cad system.
Just as an extra for item 7, you can temporarily disable intellisketch while you are sketching by holding down the ALT key.

bc

 

[KENAT]

Beach thanks for the intellisketch alt key tip. I'll add that in before I distribute it around here or turn it into a FAQ.

Revised para 7:

7. Learn to use intellisketch. As a model gets busier and there is more geometry to make relationships to, it may be necessary to temporarily suspend intellisketch, using the Alt key, or to turn some relationships off to make sketching easier.

KENAT, probably the least qualified checker you'll ever meet...

 

[PatCouture]

Great job Kenat!

 

[HDS]

This is a good list that applies to any cad system except for items 3 & 7.

SW does item 3 by default but it is very bad about letting you leave things under constrained. Pro/e never leaves things under constrained but it makes a lot of decisions you may not like.

The relationship assistant is also very useful (only for sketch not relationships with coworkers).

 

[KENAT]

HDS thanks for confirming that about SW. I've used Pro E and that's how I remembered it but my colleague claims it was wasn't an issue and it was always right.

KENAT, probably the least qualified checker you'll ever meet...