No such thing. Either will most likely work fine, but YOU need to evaluate
both of them to see which fits YOUR needs. The newsgroup can't do this for
you, but since your asking, I'll tell you... Solid Edge. UGS has their
focus solely on engineering (unlike Autodesk), they own the component
technology that is used inside both Solid Edge and SolidWorks (Parasolid,
D-cubed), and their support group is top notch (get to talk to real, live,
UGS support engineers immediately). Not to mention, Solid Edge is a great
Please tell me which of this products is beter in 3D designe.
> Which is more efficient and works better.
> What is theirs adventages and disadventages.
> Which is better and why ?
What exactly do you think PLM is? Look at UGS's portfolio of products.
With the exception of Teamcenter Enterprise (which is the high-end data
management product of the Teamcenter products and extends beyond Engineering
to the entire enterprise), everything else screams "Engineering" or is
component technology for an engineering product. UGS has always used VARs
to service/sell Solid Edge and still maintained an internal support group
for customers, what is changing is those VAR's (and more of them in the
future to support more sales/customers) will have expanded product offerings
available that they didn't have before. For instance, if a customer needs a
high-end seat of CAD, instead of walking away since they only had Solid
Edge, they can now offer NX. And the beauty of that is, they generally only
need a seat or two of NX, and Solid Edge can supplement the rest of their
needs. Both can associatively use each others files, and both are tightly
integrated into Teamcenter Express, Engineering or Enterprise.
I'm not sure what you meant by "UGS focus is PLM. Unigraphics NX is proof of
that.". NX is a high end modeling system that supports a variety of
different engineering disciplines, not just product/machine design, and it
also has modules for CAE and CAM.
I use SolidWorks, and recently had a Solid Edge demo. Its a pretty
nice looking product. If I was making the purchasing decision for our
company, I would take a serious look at it. One of the things that
stood out for me was the integrated file management addin. It uses MS
Sharepoint technology. Another feature I liked was the way it handled
large drawings. It converts the solid model to 2d lines so you can
edit your drawing faster. This is similiar to "detached drawing" in
SolidWorks, but it looks like it works much better.
I'm nore talking about UG than Solidedge. Solidedge has always been a
very good simliar alternative to Solidworks. UG, while powerful, does
little to make the product easy to use nor has the tools that are
commonly available in "lesser" cad packages. Hence my comment about
their focus on PLM. Last time met with our UG rep, he was more
interested in selling teamcenter than hearing about what UG needs to be
Anyway, Solidedge is not quite the same in this regard but it has
seemed to get the short end of the stick at UGS as far as marketing
goes. Maybe this recent annoucement will change things. Competition
between them is a good thing.
Actually, all of UGS got the short end of the stick when it came to
marketing. During the EDS years, EDS handled the marketing, and all that
they marketed was EDS. Fine if you sell a service, but terrible if you sell
a product. Now that EDS is out of the picture, UGS and the various products
should see some significant "air-time". I know what you are saying about NX
though, If you aren't GM or Ford, who are you? :)
I've been using SE off and on for a year and change. I still find it
awkward. As long as you go with the flow it is great. But get off the
path and you are in the ditch.
There are some nice features in it, but SW has a pretty good track
record of taking the nice stuff from SE and improving on it.
Stability wise it seems to favor the experienced user. Novices seem to
make it crash alot. And people with happy hands won't like it.
The whole drawing thing is one area where it does do well. Equations is
SW M> I use SolidWorks, and recently had a Solid Edge demo. Its a pretty
Still using the 2 year old version of Solid Edge (V14, current version is
I have still not figured out what you were talking about regarding the
smartstep ribbon bar not allowing edits to previous feature creation steps.
I am able to edit any previous step of any feature I create. Perhaps you
could give me an example feature and step that is un-editable?
What's the deal with equations?
Let's see. Edit a part while in an assembly and try to get back to
assembly mode. The only way I could figure it out was to close and
reopen the assembly.
When placing a part do something that gets you out of the place
enviroment and try to get back in.
Click on zoom to area. No easy way I can see to get back to what you
were doing on the ribbon bar..
Toolbars run off the window when the tutorial comes up. Can't get at
zoom, etc. without resorting to the menu.
Intellisketch is buried in a menu. It should be in a right mouse menu.
Setting up a drawing takes a visit to four different places. File
Properties for units, Sheet setup, Tools/Options/Drawing Standards, and
The way you set up a GDT box is awkward and not wysiwyg. Yes you can
save favorites but it harks back to type it in on the command line
which some may find awkward.
On the other hand, SE does a much better job of SW at setting up
SE will place a center mark on a hole in an inclined face.
The pathfinder is pretty unsophisticated compared to SW feature tree. I
have yet to find a way to roll back. And getting parts and assemblies
to update is something I haven't quite figured out.
Macros require VB and a programmers knowledge. No macro recording like
and then there is SE support. We tried to get SE17 this semester, but
they couldn't be bothered to send it on time.
On the plus side, if you can figure out how the flow works and stay
inside it sketching and the other tasks can go quite quickly. Pro/E is
he same way.
And of course the icons for commands still lack sufficient contrast to
really stand out and show whether a button is active or inactive. This
is nowhere more evident than in the place environment where one must
really take a good look to see which step is being done in a place.
On the other hand, SE has a nice way of letting you first pick the part
to be involved in a place (mate) and then pick a face on the part. This
makes placing in large assemblies much easier.
The ability to flip the sense of a place (mate) does not seem to exist
in SE. Two different mates are used, Mate and Align Face depending on
whether planar faces should mate with the outward normals opposing or
aligning with each other.
The version of SE I am using has a mate tree system similar to SW circa
They work well. SE is quite superior to SW in the area of equations.
This is because SE treats all dimensions as variables. If the dimension
has a fixed value then V274=5 for example. But you can just as easily
say V274 = 2 * V273 + 1/2*V269. Obviously, dimensions do not seem to be
tied to a particular feature as in SW. Instead of D1@Sketch1, SE
sequentially numbers all dimensions starting with the letter V. SE also
treats other information as the same type of variable so for example
one could tie a dimension to Young's modulus or the CLT for the
material specified. And SE will display the equation for a dimension
with the dimension if so desired. Editing an equation is as simple as
double clicking the dimension which replaces the ribbon bar with an
Excel like equation editing bar. I didn't find anything like a design
table in SE. Perhaps it is there in a newer version.
My conclusion is that SE will demo very well. But when viewing the
demo, try to get them to go off the beaten path and change things after
the fact or interupt the Smart Step system. Have then do some
constructions in the profile editor like a hyperbola or involute.
Change a drawing from ANSI inch to ISO and from A to D size and see
what is involved. Try dimensioning an isometric view or an oblique
view. Have then show you how to quickly automate simple tasks. And
above all have them log you into their user group and let you browse
around a while.
See answers inline:
Select "Close and Return" from the File menu or hit the ESC key.
Select the part you were attempting to place and on the ribbon bar select
the "Edit Definition" button. You now have the original SmartStep ribbon
bar that was available when you placed the part initially.
Right click of the mouse exits the Zoom Area command and returns you to the
point you were at in the previous command.
Can't help you there. Running 1280x1024 on a 19" LCD with large buttons
"on" still shows all my buttons with the tutorials running. Can do the same
on a 17" CRT @ 1024x768 with large buttons "off". Depends on how low your
resolution is and how small your monitor is. Is this really a Solid Edge
problem or a problem with the user's choice in hardware and settings.
Depends on how often you change your settings. I change them very
infrequently. You still have the choice of adding a button to the menu or
creating a shortcut key for it. Have you logged your preference with UGS as
I don't know how much you change between first and third angle projection or
between inch or metric units, but once a template is set up, none of those
areas are needed for production drafting. With the exception of Sheet
Setup, the rest should be setup in the template used. File property/Units
changes the toolbar data entry field units. Tools/Options/Drawing Standards
are things like dimension standards, third/first angle projection, how your
section line arrows are placed, basicall drawing standards like it says.
Format/Style is where you set up dimension/text/hatch styles such as ANSI,
ISO, etc... (actually those are premade but can be modified or new ones
What he is talking about is the form has an entry line and you click a
button with the graphics you desire and it puts in a control code such as
"%PO" for the position symbol, but the button you clicked has the position
sysmbol on it. In the right preview pane it shows you a dynamic view of the
feature control frame that you are placing. Saved feature control frames
will reload the control codes back on the entry line and loads the graphical
preview. Pretty straight forward.
Rolling back is called "Go to" in SE. Just right click on the feature you
want to rollback to and choose "Go To". Parts update automatically by
default, so you don't have to click any update command, and assemblies are
the same way. If for whatever reason you turned Automatic Update off, you
can click the Update All button to force an update. and in a part, right
click on any feature and choose Recompute to force exactly that.
This is something I would like to see too.
Can't comment on educational seats and your specific situation. Commercial
seats are shipped to US customers rapidly after RTM, and those of use that
do testing get it with in a couple of days. Support calls are answered
immediately by support engineers who can aswer your questions. When I order
Training manuals, I recieve them 2 days after I send the request.
If running on XP, the active buttons are orange just like in Office. Now if
that isn't a contrast from gray, I don't know what is!
Your right and wrong. Once a Mate is placed and a Planar Align is needed
instead, the Mate can be edited and "flipped" to a Planar Align. A more
efficient method would be to use FlashFit which will use the initial
orientation and apply the relationship that fits and a TAB can be used to
flip it on the fly.
And that means what? What functionality is missing?
I missed the jist of the comment. By the way, the somewhat equivalent to
design tables is called Family of Parts and is a tab on the Edgebar.
And above all get training from a certified Solid Edge Training Associate.
Some of the answers that I provided on items "TOP" couldn't seem to figure
out are basic training issues. Even going through the supplied tutorials
would have answered many of these questions. And of course, it also helps
to use the current version of software (V18).
Ken already responded to your list of issues with SE but I have a suggestion
that's probably going to upset you. You need to get your hands around some
of the most basic funtionality of SE before you continue teaching it.
You're the reason I tell people not to visit newsgroups for opinions of CAD
software. Too many people don't know what they're talking about when it
comes to criticizing the "other" CAD package.
See answers inline
That is not obvious in the interface nor in the help nor in the
tutorial where the problem first cropped up.
Again, not obvious. This should be a toggle.
Yes it is an SE problem because SE claims to be Windows compliant in
its interface. SW correctly rearranges toolbars if the window is
resized. SE has other problems with this as well.
We have no contact with UGS. We are educational and the software was
free. That has changed now too.
We use Intellisketch alot because we are doint constructions and
sometimes have to disable SE's "brains" so we can do what we need to do
without the software interfering.
SW has pretty much all the drawing info set in one place for a document
and that which is needed immediately is in the Property Manager.
Setting up a Format Style does not appear to be for the faint of heart.
Pretty confusing to a new user. On the other hand I like command line
Right...SW let's you drag a bar up and down the tree to visually see
what you are doing. GoTo is an unfortunate choice of words that really
doesn't communicate what is being done. And SW also has the right mouse
menu choice to instantly roll back to a specific feature. The
functionality is there, but the interface gets in the way.
Update, recompute, update links are terms all used for what SW would
call a rebuild. Why this is in a menu and not on the main toolbar
remains a mystery to me.
And a big source of user productivity. Judging by the number of posts
on comp.cad.solidworks regarding macros and VB this is a big area for
a significant number of companies.
Whether it is the schools bureaucracy or UGS I don't know for sure. I
do know that in my day job UG people have been extremely lax in getting
back to me. In fact it has been months since I sent an inquiry in to
the Indianapolis office. And that isn't the first time.
It took a lot of explaining the students about this point. Why change a
mate type to flip faces?
This isn't an issue. If I can get a CSWP without taking formal training
and yet can't figure out the basics of SE after all this time, well,
maybe you are right, add training expense to the cost of the software.
Without an open user forum there is little chance to get questions
I apologize for my earlier post criticizing your knowledge of SE. Using
both SE and SW would be equivalent to speaking 2 languages and I doubt I
would be any good at it. I can't take it back so I'll offer you a couple
more tips to help you teach the class. Because you're still on V15 some of
these may not work. I can't remember when they were implemented.
- When creating sketches hold down the ALT key to override Intellisketch
- Use the CTRL, SHIFT, & ALT keys in combination with RMB to take care of
all your windown maniupulations. This will keep whatever command you're in
at the time active and once you get used to this method I doubt you'll ever
go back to the toolbar again. CTRL + SHIFT together is required for
- You don't need to change the mate type to flip faces. If you flip a mate
relatioship it will be automatically converted to a planar align. If fact
any time you choose a mate relationship SE will automatically convert it to
a planar align if that is what it should have been.
- Update Links and Update Relationship commands are in the main toolbar.
There's no need to go to the menu.
- Almost any tool you need can be added to the toolbars if you want.
- MOST IMPORTANTLY if you are at all serious about improving the efficency
of you and your students in the use of SE then visit the newsgroup. If
you're teaching it then you should have a Sold To ID that will give you
newsgoup access. Whether it should be open to the public is another debate,
but if you have access and not using it then you're ignoring one of your
Again sorry for the criticism, it didn't belong on this newsgroup.
Thanks. I don't want to be unfair to SE and I appreciate the help.
Knowing two languages does open the eyes.
Ken sent me info on the student portion of the UGS newsgroup. There
wasn't much activity there, but I'll keep it in mind.
There may very well be a Sold to ID somewhere in the bureaucracy, but
I don't have it.
I don't just want ot override Intellisketch, sometimes I want to change
it's preferences when working in close.
I understand I've wanted that functionality a couple of times also. What I
was getting at was that it's much faster to hold down Alt to override
intellisketch then apply the desired constraint rather than keep changing
the settings in Intellisketch.