The BIG Question: SW2004 or SE14? 1

[HomeMadeSin]

3 years ago, I evaluated Inventor, Pro/E and SolidEdge. Although I made the choice to go with Inventor partially because of my familiarity with AutoCAD - that has since proven to be a fateful mistake. The other programs import/export and handle dwg files BETTER than Inventor. I did like SE the best, but chose wrong.

Now I am switching programs. I've tried Alibre (don't go there), Vellum Cobalt (yeah, right), MDT (no way), Pro/E Wildfire (I'd have to sell my left you-know-what to pay for the training), SolidWorks 2003 and SolidEdge 14.

For my needs, serious lofting, sweep and surfacing is required about 50% of the time (pump design). This is where Inventor really flubbed. SolidEdge 14 seemed to have the best surfacing capabilities, to be honest. I still like it the best but it seems that SolidWorks has the best overall package: CosmosExpress, PhotoWorks, FeatureWorks, and a whole host of partner package options. And SW appears to be truly the 3D standard in terms of the amount of users. Plus, it seems that EDS is selling their MCAD software division.

If SE had the goods like SW, it would be close but I think I could make it happen. But I made a choice against the grain 3 years ago and I don't want to do it again!!!!!!

So I need honest comparisons between SE & SW. Anyone?

 

[PatCouture]

Hi

I've gone through the same problem 3 months ago. I was working with MDT6 for two years and I've finally been able to convince my boss that we needed something a lot more powerful than MDT crap.

After some research and reading on the net I decided between SW and SE, to go with SW and then started working with a copied license just to see if I was right. The interface is good and intuitive. You discover a lot of "wow" command, that impress and that are useful, but there is also a lot of can'ts in the program that make you go through a long way to do what you want. For example with sheet metal, SW will let you do whatever you want even if it's impossible to do in real life, and for welding don't even think about using it.

After two months with SW I made some really cool stuff with some drawing but other things were a real pain to adjust. And a friend of mine who was working with SE made me take a closer look to SE.

I talked to some people who worked with one or another products and each time everyone is satisfied with his program it's a mather of taste. One of them had worked with SW for six years before switching to SE, so I asked him if SE was able to do all the amazing things the VAR of SW was telling me that SW was doing and SE was not, and beside EDrawings and CosmosExpress, you can do everything SW do with SE. the only things is that SW put all his efforts on selling his products and SE put his efforts on developping his products. So SE can do it but won't scream it to all the world, they tell it only to their users.

So two weeks ago I took a formation on SE V14, and I've seen really what SE is about and if you're serious about what you do go with SE because the program can do about everything you need and he helps you do it in a productive way. Especially if you want to do large assemblies SE as all the tools you can think about to help work with thousands of pieces. And the Drafting is way better in SE than in SW. I also realize that SE as always a little option or fonctionnality that make you realize that the developper are listening to their users.

In resume, I'm convince that for me SE is the best, but there is also some other people who prefer SW. So check carefully the two products and don't just base your evaluation on what the VAR is saying make them do it and showing it and you'll see who is selling and who is helping.

That's what I realized the last three months.

I hope it helps. And good luck

Patrick.

 

[PatCouture]

I forgot to tell you about the sufacing capacities of SE, with blue surf and blue Dot, SE is the best and even if the peoples of SW tell you the opposite SE is way up in that category.

Patrick

 

[swertel]

Solid Edge is definitely the best in the market for surfacing, currently. I really want to stress CURRENTLY because the market changes so quickly. Granted, that comparison is only based on the packages considered to be "mainstream" or "mid-range."

Personally, I feel the drafting is better in Solid Edge. I like their tech support structure much better, also. As far as solid modeling capability, I would say SW and SE are even. They can each do what the other is doing, but there are different workflows to get there, which brings me to my main point.

What is your preferred workflow?
I liken Solid Edge and SolidWorks to TI and HP calculators, respectively. I can not use HP calculators because of their "reverse polish notation." My brain just doesn't think that way. Likewise for SolidWorks. I don't want to have to start with a sketch, I want to make a protrusion. Tell me what I need to make a protrusion. Don't have me make a sketch or 2 or 3 and hope that I created them correctly in order to create the actual feature. In Solid Edge, you tell the software what you want to do, and it tells you the steps that you need to take in order to define that feature.

So, now that my bias is obvious, I realize that you won't consider Alibre. I assume it is because you need surfacing functionality, which Alibre doesn't have. If that is truely the case and you are immediately going to be purchasing software, then go with SE. If you are going to be waiting another 6 months, then review SE, SW, and Alibre again at that time because the new releases will be out or close to out and the game will have changed.

By the way, to temper my bias, I will just mention that I have used: CATIA, UG, SolidWorks, I-deas, and Solid Edge in production environments and I am currently proficient in Solid Edge, followed by UG, then Solid Works. I'm training myself on Alibre. I haven't used CATIA or Ideas in 3+ years.

--Scott

For some pleasure reading, try FAQ731-376

 

[jgfrankusa]

Greetings:


Even though I don't fully know SE v14 capability at this point yet; however here is what I found during couple of days test drive to model connector parts (mostly involve in solid modeling and sheet metal). Please correct me if I am wrong.

1. SE doesn't recognize a sweep bottle profile edge as a triming edge to trim LabelSweepProfile.

http://home.comcast.net/~wangphk/SE/Bottle.jpg

http://home.comcast.net/~wangphk/SE/BottleLabelSweepProfile.jpg

2. I can not select multiple text profile for a normal protrusion or cut-out onto a cylinder surface.

For instance in order to protrude "MADE IN USA"
onto a cylinder surface. First, I have to select M curve -
select Curve chain - Accept - Select Cylinder face -
Select direction - Finish and repeat the whole process
for the rest of the string (12x6=72 mouse click!! There are 9 character + 3 pocket).

3. I can not accurately draw a cross section line/plane.

http://home.comcast.net/~wangphk/SE/3-1.jpg

http://home.comcast.net/~wangphk/SE/3-2.jpg

For instance, with intellisketch turn on, SE show a Midpoint, Center point etc; however, when I move the pointer away , there isn't any tracking (similar to sketching a profile where a dash line show the endpoint line up with other point or like the sketchpoint) that could tell me the Section plane is aligned where I want it exactly to be.

4. In some circumstances, dimensionning is so cumbersome and time consuming (require too many mouse click).

For instance, to use a Symmetric diameter dimensionning. I need to Select Symmetric Diameter - Select Hor/Vert, 2 Point etc. - Click on Half or Full Icon - Select Axis of revolution - Select Profile entities - Place the Dimension - Click on select tool - Select Dimension text - Drag it above or below the Axis of Revolution - Select the Leader and turn it to either inside or outside. In comparison with other MCAD package, it has only one dimension button instead of 8 main (not counting options in the smartstep toolbar) and the Diameter dimension can be done 4 steps max. Select the axis, select the edge, select the axis again, position the mouse pointer where ever you want and place.

5. Doesn't support mouse wheel as zoom in or out feature.

In Pro/E (Wildfire) or SW, I can use mouse wheel to zoom in and out at all time.

6. SE can not bend a sheet metal with feature like bead, louver, dimple etc.

http://home.comcast.net/~wangphk/SE/6.jpg

For instance, I create a rectangle flat pattern sheet metal with a default bead feature. I try to create a bend accross the flat pattern and the bead, it failed. Only Pro/E can perform this so far.

7. Can't create a drawing while the model is currently open in Part mode. It will generate an error.

8. Modify a dimension in draft mode doesn't change the model. So it is not fully associative.

http://home.comcast.net/~wangphk/SE/8-1.jpg

http://home.comcast.net/~wangphk/SE/8-2.jpg

9. Drawing doesn't update automatically when part has been modified.

10. After mirroring a sketch profile, user needs to connect mirror endpoints together to validate the profile. Otherwise SE will generate an error message saying that the profiles need to be closed.

11. Doesn't have local cross section.

http://home.comcast.net/~wangphk/SE/LocalXsection.jpg

We usually need to create a partial cross section to see inside the connector.

12. Can't convert solid modeling to sheet metal part.

Sometimes it is easier to create a solid modeling with all the bend feature then convert to sheet metal

13. Can't create a variable patterning feature.

For instance, in Pro/E I can pattern any feature (cut, protrusion, hole etc) which varies by depth, width, height, angle etc

14. Can't create variable round feature.

http://home.comcast.net/~wangphk/SE/14-VariableFillet.jpg

All come down to this, it all depends on the application. For connector design, my hat goes over to Pro/E (Wildfire) first, SW second and SE third. It would be a perfect world, if I could have Pro/E for Solid modeling, SM and surfacing, SE Express route for assembly requiring hose interconnect and cable harness, SW for presentation (Photoworks), friendly user interface, easy lofting, round, sweeping etc all in one package.

 

[swertel]

Hey JGFrankfrom the USA,

You bring up some good points, but a few of them seem to be based on comparison to the logic behind SE vs other CAD packages. Allow me to shed some light on the "why we think it works this way" so we can all learn from it, for those that I know, anyway.

1) Haven't ever tried this, but there are more options now in v14 that would allow you to what you want, but it may require more construction geometry to get there. For example, try "including" the curves that you want to trim to into your sketch of the circle and then make those included sketch elements "construction/reference." You may have to create other intersection curves or projected curves to include. All will remain associative.

2) Yes that is a PITA. Don't forget that you had to start out by creating a plane outside the cylinder to create a sketch on with profile text elements in it and project those onto the surface to create the curves that you can protrude normal from the surface.

3) One of those bugs that will never get fixed. When creating your section line, the intellisketch and autoconstrain do not actually constrain the elements, even though it appears that it does. First, make sure you have "Maintain Relationships" checked and then create your cutting plane lines. Add the connect relationship to the center of your mounting hole to the cutting line. Explicitly adding the relationship is the only way to actually create/keep one when defining the cutting plane. Don't forget about the "revolved cut" option in the Ribbon Bar when creating your section view.

4) Yep. They started to stream-line the dimension function by adding yet another dimensioning tool, Smart Dimension. It's not too smart and isn't any easier to use.

5) Don't know. I use a SpaceBall. If you can afford one, try it, you'll like it.

6) Don't do much sheet metal work.

7) What is this error? If you have maintanence, log it. I don't get this error.

8) When you install SW, you have the option of disabling the modification of parts through the drawing. Most users I know prefer this method so they don't accidently change a model while dimensioning, especially when you often have to add extra text or tolerances to the draft display. Also, it keeps drafters from changing the model that an engineer built. Finally, if the draft file had control to change the model from from it, then the model file would always have to be loaded into memory of the machine doing the drafting and lock it in-use to that user. Therefore, the drafter and engineer can't work concurrently on the model and draft file. I did like the convenience of being able to tweak dimensions while in the draft, but all-in-all, switching back the part is not a big deal unless you suffer from the error described in item 7.

9) No it doesn't, nor should it. When you change the model and open the draft, a gray border appears around the drawing views. That tells you that something in the model changed. If it wasn't supposed to change, you have the luxury of not updating the views and going to the model to see what changed. Likewise, you can update the models and the drawing view tracker will list any dimensional and some annotation changes. It boils down to having an extra security measure from someone accidently changing something they shouldn't. When dealing with in-place editing from assemblies or inter-part copies, accidental changes happen quite frequently if a file management system is not in place (not refering to PDM).

10) Sometimes yes, sometimes no. I haven't quite figured out when it will connect them and when it won't. Either way, it's annoying.

11) Look up the help for Partial Section. It's new to v14 and will do exactly what you want. Compared to other CAD packages, this is the best rendition of how to create local cross-sections. Modifying them, that's another story.

12) It's funny that you can go from sheet metal to part and back again, but not part to sheet metal. I get around it by creating a small sheet metal tab as the initial (base) feature and then transferring it into part. Within part, my first feature will consume the small tab I created.

13) Nope, you can't.

14) You can create variable fillets, blends, etc. I don't know if you can do what you show there, but variable fillets are possible.

--Scott

For some pleasure reading, try FAQ731-376