OT- Solid edge learning curve vs SW etc..

If you go the export route use STEP instead of IGES if at all possible you might regret using IGES there tends to be alot more loss of data through IGES with solids.

Corey

You're better off working natively if you can. SE and SW are close enough in basic function that you should be able to do basic modeling in SE immediately after maybe working through a tutorial.

Translation is an ugly business, and although SW is getting better at handling imported data, there is nothing like working native.

matt

clay wrote in news:vQ0ud.7122$ snipped-for-privacy@news01.roc.ny:

And then you'd have to translate it back as well and then check & fix it, right?

Strangely enough I am in a good position to advise you on this since I am a CSWP and have been attempting to learn and then teach SE to others. I have been learing SE since September and still have a hard time getting used to it.

You are going to be very frustrated. The following differences will quickly become apparent:

1. Getting fully constrained profiles can be extremely frustrating because SE has built in intelligence that will either do things you don't expect or make it impossible to do things you want to do. Many times you have to change settings in Intellisketch in order to pick the correct entities for a given constraint.

1. Troubleshooting contstraints in sketches can be very difficult because the only information you have on constraints are symbols that are placed on the sketch elements, many times one on top of the other. A lot of the constraint troubleshooting tools in SW are just plain missing.

2. SE will force you to work one way, its way. In addition this is done via the SmartStep feature implemented through a Ribbon bar. A Ribbon Bar is somewhat a cross between a toolbar and the Property Manager. As you create a feature certain commands in the Ribbon Bar will become active or inactive. If you miss a step or an option and go on to the next step you will find that it is difficult or impossible to go back and set the missed option.

1. Menus are not an alternative to the Ribbon Bar and Edge Bar commands for creating features.

2. Some things that you do in a single command are broken into two commands in SE. For instance to create a section view you must first create a cutting plane and then use another command to create. The same two step system is used for creating a symmetry plane for automatic symmetric constraints.

1. Because menus do not play an important role in duplicating commands for features or sketch entities you must rely on a series of icons, many of which are not obvious in their meaning or are hidden in flyouts. To definitively know what an icon does you must look at an ennuciator on the screen that gives the function. This ennuciator is activated by placing the cursor over the icon. In addition many icons won't appear unless SE thinks you need them.

2. The help is very sketchy and it is difficult to find information or even enough information to create certain features. And of course SE uses a lot of terms differently than SW making it harder to find what you want.

1. Doing the tutorials is probably the best way to learn how to use it. If you can get a hold of the training manuals they will also be a big help if you can get through them. Since SE is so dependent on the order in which you do things and the tutorials demonstrate (but don't necessarily explain it) you will get up to speed quicker.

2. I have found that Feature Works does a fair job of converting SE parts to SW feature based parts. You milage will vary here.

1. Setting defaults for a part or drawing and getting them to stay that way can be difficult because the menus for doing this are several and varied in location.

2. Assemblies will be another experience for you because mates are done purely through an iconic interface and results can be very much order sensitive.

1. Picking what is mated to will be new experience for you because many times you have to pick the object and then the face, two steps where SW has one.

2. Transfer geometry with Parasolid, not IGES please.

1. If you get SE make sure it is a stable service pack. You think SW has problems.......

In summary, I have been trying to learn SE for four months. I can build most things that I can do in SW but I find the user interface to be clunky, quirky and unforgiving. It is SE way or the highway.

This is very interesting, Paul, and I appreciate you taking time to write it all down. If it were someone whose expertise and intelligence I didn't recognize I'd be tempted to wonder if they were just prejudiced to SolidWorks and not necessarily giving Solid Edge a chance. But knowing you I would presume that you've analyzed the problems you mention carefully and that you've tried to be impartial. There was a time when I had to choose between going independent with Solid Edge and going independent with SolidWorks. Obviously, I chose SolidWorks, and whereas there has been more than a little frustration along the way I'm fairly satisfied (and gratified) that I made the right choice.

Now if we could just get them to provide a little more value for the yearly maintenance fee.

Best regards to you (and all), 'Sporky'

intelligence

prejudiced

Placing constraints manually does not typically require the use of the intellisketch options unless you have turned off a "keypoint" locator such as "endpoint". I can only think of one scenario I have encountered where Intellisketch needs to be changed: Ane intersection is desired between two lines and the midpoints of one or both lines are also at the intersection. In this case, the midpoint is found first if the instersection filter is turned on. In this case, the midpoint filter will need to be turned off. The beauty of Intellisketch is that when drawing the sketch it is placing most if not all of the geometric constraints needed to constrain the sketch and it does this using alignment indicators and tooltips so there is constant feedback as to what it is doing.

other.

Constraint troubleshooting is not difficult at all because you can look at the sketch entities and instantly see what constraints an element has on it (such as a horizontal line, it will have the Horizontal constraint located at its middle). Since there are different symbols that mean different things, it isn't a problem when a couple overlap because they were designed to still be distinctive when they do (such as a Endpoint Connect and a Tangent at the same intersection. The Connect symblol (a box) is clearly seen inside the Tangent rlationship (a circle). If there is a question of what the parents of a constraint are, the constraint can be selected and it's parents will highlight.

This is incorrect. The reason that the smartstep ribbon bar is there is to provide instant feedback as to what step of a feature you are in, and if you did miss something, you can click on the button representing the step missed and define the input. It is so flexible (and the norm is to apparently start over in other products) that the training even stresses resisting the urge to delete a feature if you put in incorrect parameters, but rather use smartstep and revise the parameters and then complete the feature.

commands

True. Menus contain lesser used commands as they require more navigation to use, but all menu options are available as buttons :)

True on the cutting plane/section view, untrue on the Symmetry constraint. The Set Symmetry Axis is used to respecify a different axis if needed. If one has not been defined in the sketch, the Symmetry constraint will allow setting the symmetry constraint. The Symmetry constraint is only usefull if both sides of a symmetric sketch has been defined. If you don't want to go through all the work of drawing both pairs of sketch entities, one can use the Mirror command with the Copy option set to complete the second half of the sketch and build the symmetry relationships all with one command.

commands

It is true that toolbar buttons are the heart of Solid Edge (and every other application designed from about the mid 80's forward). As far as the icons that don't appear "unless Solid Edge thinks you need them", I would like to see you put a Cutout in air. Solid Edge blanks out the icons and menus that are not applicable for a certain operation or state of a model to reduce command clutter, such as disabling all the material removal features when there is no solid present in the file to remove material from.

And I thought the Help was rather good :)

several

Order sensitive? You will have to explain that one in detail since the

3D constraint manager is the same one that Solid Works uses and solves the constraints in parallel.

Solid Edge has a option for this. Turning on Reduced Steps will allow picking just the face. The reason for the options is that if an assembly is loaded with Lightweight parts, the act of selecting the part first loads it fully into memory (Active/Inactive parts).

Yes, if you think Solid Works has problems, it is not alone but it also is not any better than Solid Edge when it comes to stability. I also wait to move my users to a new version till about the second service pack.

And I could say the same about Solid Work, Inventor, Pro/E, UG, Catia, Ideas. They all have their peculiar workflow and it is all foreign if it isn't what you are leaving behind (or haven't left it behind).

Ken,

Not really bud,,, I've used Ideas, Pro-E, UG, even a bit of Catia 4. All have very explicit, cast in concrete, proceedures that you must follow.

Solidworks is totally the opposite. You can litterally work any way you want. In fact, It's so open and unconstrained, you can do things you really shouldn't. This can be hard on newbies, but most people learn the do's and dont's pretty quick. Once this is accompished, what you're left with are allot of options. No other system like it, not even close.

Regards

Mark

Thanks Ken. I appreciate the appreciation.

I'll have to say that if SE is so difficult to learn that it takes the paid training and certification to use it that there is something wrong. I was certified in SW without formal training. So I ain't dumb. I 've used Pro/E, Anvil and CADAM extensively and if SE requires the training and experience necessary to use those programs there is a problem.

If you think those are bad try Mechanical Desktop. 8~) You really aught to take Pro/E out of the category. Nothing hard about it these days unless you're trying to pick it up starting with zero 3D experience.

Paul,

Gotta agree there. I was doing productive modeling in SW in a couple of hours, comming straight from Pro. People that have never used it have a very difficult time believing this, but it's true.

Regards

Mark

I'd second this. It was very easy to learn SW coming from ProE. I learned ProE very quickly as well. My father taught it to me as a kid.

Regards,

Sounds like a lot of SW users in this NG .

Sorry. Didn't mean it to come across that way. Just trying to say that you obviously know Solid Works very well and have the certification to prove it. Since you have only been at Solid Edge for 4 months, and I assume that is part time as you are still using Solid Works, and you don't have Solid Edge certification yet as you do not know it quite so well. I can judge from some of your comments about SE that you are not using V16, and you are still biased by your SolidWorks background.

Learning another CAD system is like learning a different language. For instance, you know English, you think English, and it comes without any effort whatsoever. Now you decide to learn French. You start out comparing every word to it's English equivalent and think English when trying to build Sentences. Eventually it becomes easier, but without complete immersion, you are still thinking English when trying to speak French.

Any ways, I'm sorry that it came across that way.

Ken

Clay's original question was how long will it take him to get up to speed in SE to do some minor modeling work. If Clay works through the tutorials he should acquire basic skills in relatively short order. But he is going to miss a few features that SW has always had and that we take for granted.

Just this even> Sorry. Didn't mean it to come across that way. Just trying to say that

Node news is good news.

It is actually in Help and it is simple enough that there is no need for a tutorial. Check for the topic in help as "Parts Lists" or "Parts List Command". Another terminology issue :)

Further confused by the help using the term BOM for a Bill of Materials that is saved to a file from an assembly and not having a cross reference for the two terms. This part of the country almost exclusively uses the term BOM (except I would guess in SE shops).

SE is full of these simple assumptions that can take hours to figure out.

SE is not the only app. that uses the term "Parts List". Inventor and UG NX also use the term. I'm sorry you spent so many hours looking for it and never found it.

I would be looking for the Parts List command in Solid Works and wouldn't ever find it, but wouldn't be a problem in Inventor or NX.

It's just a matter of where your origins are.

Kind of like calling a sugary carbonated drink "Pop" in the North, and "Soda" in the South.