Have a customer that has Solid edge & SolidWorks. Older data was created
in Solidedge. Having never used it, I need to do some minor design work
in solid edge. I have 7 years experience in SW in addition to tons in
other surface/solid modelers. SDRC, PRo-E, CV etc... How long is it
going to take to come up to speed (just doing basic modeling, drafting)
in SolidEdge? I have an existing SolidEdge assembly that need minor
revisions (holes, part redesign etc)
Or am I going to be better off just exporting Iges files, and creating
changes & drawings in SW?
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.
clay wrote in news:vQ0ud.7122$ firstname.lastname@example.org:
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.
2. 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
3. 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.
4. Menus are not an alternative to the Ribbon Bar and Edge Bar commands
for creating features.
5. 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
6. 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.
7. 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
8. 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.
9. I have found that Feature Works does a fair job of converting SE
parts to SW feature based parts. You milage will vary here.
10. 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.
11. Assemblies will be another experience for you because mates are
done purely through an iconic interface and results can be very much
12. 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.
13. Transfer geometry with Parasolid, not IGES please.
14. If you get SE make sure it is a stable service pack. You think SW
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),
I wouldn't be to sure about the impartiality. Solid Edge has their own
user certification and he doesn't have it, and it is apparent that he
doesn't know it very well, nor is he using the current version.
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.
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.
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.
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 :)
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
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).
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.
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
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
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.
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.
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 evening I tried to put a BOM in a drawing. Seems simple enough.
But there was nothing in help on how to do this nor in the tutorials. I can
tell you how to get a BOM from an assembly into a text file, but not into
the drawing. SE14 is only two releases back. Either they have covered a lot
of ground since then or there is another skill that I just plain couldn't
find in help or the tutorials.
Node news is good news.
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
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.