Sketching & drafting commands 2

[BeefMarinade]

Hi,

I'm currently evaluating SolidWorks 2003 for the company that I work for.

We come from an AutoCAD & MDT background, and we have become used to certain features and commands.

Whilst many things in SW seem very powerful and easy to use, I am currently struggling with 2D sketch creation.

I'm quite used to ACAD's commands like offset, creating circles from 'tan-tan-radius', being able to easily draw lines to tangents, and being able to trim or extend to a particular line.

I currently do not know how to do this effectively in SW.

I am in a bit of an odd situation. As I am evaluating the software, I do not have any books (only the in-software help), and have not had any training.

While most things have been easy enough to figure out, 2D sketching still eludes me. I have had to resort to sketching in ACAD, and copying it into SW.

Can anyone give me some pointers? Is there a group of commands I haven't seen yet?

Also - yes, I have used the 'SW 2D Emulator' (command line for people with ACAD background), but this appears buggy(?), and seems to be more hinderance than help.

Any help would be greatly appreciated.

 

[Urb9]

khm? i can't immagine where is the problem.
In my sketches i usualy don't need more than 5-10 elements that are "thrown" on the sketching plane. Then i use geometrical constraints to order them as "object snap" works in ACAD or use dimensional constraints to ad dimensions. Use mirror and step&repeat option for simmetrical sketches...

Sketches must be simple!

 

[pegleg]

My suggestion would be to go through at least part of the tutorial. Parametric sketching kicks %&@ compared to what you're used to. Don't be intimidated by it because it is totally different. I come from a CadKey background which is very similar to Autocad.

The tutorial will really teach you a lot in a short period of time.

Steve

 

[Morglisn]

I'm fairly new to SW myself, but I may have a few pointers for you. Forgive me if I oversimplify.

First, make sure you have the toolbars you need turned on. A picture's worth a thousand words, especially when learning this stuff. Turn on Sketch, Sketch Tools, and Sketch Relations. Both the offset command you mentioned, and the trim/extend tool are there. The trim/ext. is a bit different than what you're probably used to. To trim, use the scissors icon, then click once on the piece you wish to trim. Do NOT click on a guide line, it doesn't work that way with SW. To extend, click on the line you wish to extend, then drag it to the boundary you wish it extended to.

The offset icon is basically two offset lines. This one should be fairly self-explanatory.

And, finally, as for tips for drawing circles... well... I draw mine in what most would consider an odd, strange, inefficient fashion. But I love it.

 

[DetroitPickles]

Some more "tips". If your toolbar for Sketch Tools IS turned on, are all the icons you want on there? There are a few of the possible commands, that are not shown in the default Sketch Tools toolbar. If you look in the Tools pulldown, under Sketch Entity and Sketch Tools, you will see all of them.

If you want to add some more, you can use Customize form the Tools pulldown, or right-click on all toolbar and select it from there.

My experience with AutoCAD vs. SW users (I am one) is that a sketch will take you longer to create than it would in ACAD. In ACAD, you probably had a bucket full of LISP routines to help you, and you didn't neccessarily have to "define" the sketch. BUT, I may be blasted for that.

I prefer SW's (or Pro/E's) method of creating 2D sketches over ACAD. Color coding and others are very helpful...if you give them time to sink in.




Mr. Pickles

 

[TheTick]

tan-tan-radius = "Tools-->Sketch tools-->Fillet"
also available on the sketch tools toolbar.

There is a command to extend a line to the next intersecting line "Tools-->Sketch Tools-->Extend". The icon does nt appear on the sketch tools toolbar by default, but it can be added in the customize menu.

I find that most of my students (mentoring is part of my job along with everything else) learn faster if they turn automatic relations off and manually add relations (at least for the first couple weeks), sothat they become familiar with the "unseen" constraints in a sketch.

Gravity is a harsh mistress.

 

[DetroitPickles]

TheTick,

Exactly right on the Automatic Relations statement. While I don't have it turned off, there are times when I do draw it "wrong" (lines don't touch, etc.) and make the relations myself, so I know what I have.

Also, if you turn ON "Display Entity Points.." from the System Options | Sketch options, you can learn a lot form them little dots too...


Mr. Pickles

 

[TheTick]

You won't hear this from me that often, but here's one thing that I wish was more Pro/E-like....

Sketches in Pro/E display symbols to show sketch relations (i.e. "T" for tangent, "V" for vertical).

Gravity is a harsh mistress.

 

[MadMango]

You get those little symbols in SW during sketching (plus a whole lot more), I use them all the time.

The pointer changes to add small symbols.
Tanget= T
Parallel= ||
Vertical= V
Horizontal= H

Orange Box= Endpoint Coincident
White Box= Endpoint Not Coincident
Midpoint= box with a line through it
Intersection= 2 crossed lines

...and more. Look in SolidWorks Help Topics under Pointers>Relations.

Ray Reynolds
Senior Designer
Read: faq731-376
"Probable impossibilities are to be preferred to improbable possibilities."

 

[DetroitPickles]

Yeah, but in SW you get to see these "symbols" only when creating the relation. In Pro/e, you can see them even when you edit the sketch...



Mr. Pickles

 

[Regg]

Just to add my two cents. You can use the trim tool to extend a line instead of the extend tool. Just select the line, keeping the select mouse button down, move the mouse cursor to the line or whatever you want to extend the line to, then release the mouse button.

When you select a line, information about the line is displayed in the property manager. Also double clicking on a line or circle gives some information about it and lines and circles that have relations to it.

Regg

 

[BeefMarinade]

Thankyou for all your help.

I should apologise - I can create basic sketches without problems, it's the advanced stuff I was struggling with. I wasn't clear enough in my initial post - sorry.

I think the penny has now dropped. I'm starting to understand some of the fundamental differences between MDT & SW.

I think I need to do some toolbar customising, and read up on those pointer symbols, and then I think I'll know most of it.

I'm in an unfortunate situation where it appears my sketches need to be fairly complicated (over 100 entities). I think this is the main reason for my problems.

MDT allows me to sketch that stuff with ease, but SW doesn't seem to like it that much. MDT seems to have more powerful sketching commands (essentially AutoCAD commands), than SW does.

Don't get me wrong though - SW makes up for it in other areas!

Well, I don't intend on starting any MDT vs SW debate, so I'll leave it there!

Thanks again!

Oh, and Regg - that's really handy - thanks!

 

[brengine]

This may be a dumb question, but you are doing the 2D sketches in a Part (i.e. ~.sldprt) file, right? Don't do any sketching in a drawing files (i.e. ~.slddrw), at least until you have to (which you eventually will). But for most drawings there is no need to sketch in the drawing file.

For now I'd suggest breaking up your 100 entities into separate features (extrude, cut, extrude revolve, cut revolve, swwp, cut sweep, etc...), each with their own sketch. And try to keep the sketches fairly simple, it's easier to build and edit later on.

Ken

 

[BeefMarinade]

Yeah, I'm sketching in the part file. I'm not THAT new!

I could break it up into seperate features - but I don't want to in this particular instance.

In this case, it's actually easier for me to use a big sketch. These parts are already drawn as sectioned 2D views in ACAD. From there I can edit them in ACAD, ready for SW. Then it's simply 'copy & paste'. This saves me a lot of time, as I don't have to draw it all over again...

I understand that it may be easier to edit later on, but the parts in question have been around for a couple of decades, and aren't changing too much these days - so I don't care too much.

It might sound really ugly, but I used a similar method in MDT at times, and I haven't really had any problems.

My original question was just to see if there were more sketching commands than what I knew of, or better ways of using the commands I was already using. I now have an answer, so I'm now concentrating on assemblies and creating production drawings.

Thankyou to everyone who took the time to respond.

 

[Timelord]

BeefMarinade,

I too, made the switch from MDT to SW. Here is my $.02 worth. In MDT, I always constructed my sketch to true size using the old ACAD commands like offset, array, etc. In SW it is much faster to draw a rough sketch and then dimension and constrain it. This was a hard habit to give up. It took me a long time to get used to this. When adding the dimensions you must watch the order you place them to keep the sketch from drastically distorting. SW has great sketching tools when used in this manner. The pointer changes to indicate snap points and a directed snap is a right click away. Adding constraints is also easier, but I have never been able to figure out the functionality of the thumb tack in the constraint window, mine doesn't function the same as the thumbtack in the assembly mating window. Perhaps someone else can explain its functionality.

Timelord

 

[SBaugh]

If your using SW03 and you have one big sketch, why don't you use Contour Selection? Yes you have to still break it up in to separate features, but you can use one sketch to make it. Actually it's pretty slick.

Regards,

Scott Baugh, CSWP
3DVision Technologies

http://www.3dvisiontech.com

http://www.scottjbaugh.com

faq731-376
When in doubt, always check the help

 

[BeefMarinade]

Timelord - It's nice to know that I wasn't the only one using MDT that way! Yes, I'd like to use SW the 'proper way' but it's still early days for me - I'm still on the evaluation copy... It's something I'll try to pick up if we buy SW. 'Hard habit to give up' - what an understatement!!

Scott - I have used the Contour Selection Tool a few times, but I'm not sure if I'm using it in the intended manner, or to it's fullest extent. I've tried searching the help, but it didn't tell me to much. All I have used it for, is to see how long the red 'chain' of entities goes. When the red stops, thats where there is a flaw in the sketch. I'm still not sure if that's it's intended purpose...

I hope that makes sense!

 

[DetroitPickles]

Something I HAD to learn in my Pro/E certification days that was mentioned here earlier, but may need repeating.

When sketching in SW (or alot of them), you may want to exaggerate your sketches, so some automatic relations are NOT set for you. Dimension and set the dimension value later. Sometimes I make the "exaggerated" sketch, place the dimensions without correcting them, and close the sketch. THEN I Edit the Sketch and change the dimensions values. They won't "rebuild" themselves until the sketch closes or you do a Ctrl-B or Ctrl-Q...



Mr. Pickles

 

[odmullen]

It's often useful, when doing a large or complicated sketch, to start with a simplified bounding outline, either in a separate guide sketch or in the feature sketch. Dimension it to set the overall size, then start working in the details. This will help prevent annoyances such as fillet radii that invert into loops (I don't understand why the software doesn't inhibit that yet) and dimensions that get reversed.

 

[StarrRider]

BeefMarinade

When doing large complicated sketches, I’ve found that it is usually beneficial to first accept whatever value each dimension has. Then, after the basic shape is defined, to start changing the dimension values until everything is correct. When changing a dimension screws up everything, do a Ctrl-Z (Undo), and try creeping up on it. It shouldn’t make any difference, changing a dimension in one shot (from 3 to 5) or in 4 steps (from 3 to 3.5 to 4 to 4.5 to 5), but it does.

Large changes give SW the opportunity to screw up in a big way.

Good luck

Lee

It really IS as bad as you think, and they ARE out to get you!