SolidEdge vs. SolidWorks

[Jaylin Hochstetler]

I know this is a controversial subject, but I'm curious what y'all have to say. We are actively looking into SE and I would love to here some of the pros and cons.

What are some of the pros and cons?
What are some of their good points and bad points?
How do their workflows compare?
What features does SE have that SW doesn't? (to mention some I know of: synchronous technology, dimension tracker in drawings, a built in low end PDM w/ all licenses, you can wait to update your drawings so if a DV loses a reference you can still save the drawing as a rev. before updating, and they offer a better CAM and Illustrator.)
What features does SW have that SE doesn't?
How does their sheet metal design/workflow compare?
How does their weldment design/workflow compare?
How do their assemblies compare?
How does their multibody part design/workflow compare?
How do their drawings compare?

These are a couple of comparisons I could think of, feel free to add to it.
I personally don't have any experience w/ SE but I'm sure some of you others do and can contribute to this.

[matt]

Solid Edge from the early days was known for mainly sheet metal and drawings. They have always done a good job there, and still do. In more recent years, Solid Edge is better known for synch tech and convergent tech (which means basically the ability to deal with mesh-based data in several ways). You can tell that the SE folks are more focused around machine design. You'll run into more of that type of user, and less of other kinds.

SolidWorks has typically been about ease of use. That is good and bad. You can get yourself into a lot of trouble easily if you don't know what you're doing. They also tend to be a little bit flashy, flamboyant, or whatever you want to call it. SolidWorks marketing was always a machine.

SE marketing gained the reputation of "the best software you've never heard of". But frankly, that's an internal struggle with SE vs NX, and not even so much the software as the internal organization. SE often gets the short end of the stick in internal battles. Unfairly so, I think.

SolidWorks often has many ways of doing the same thing. Solid Edge tries to be more structured in their workflow (more than likely with just a single way to do something). The SolidWorks interface is more "verbose", while Solid Edge interface typically uses fewer words or text, and it is more streamlined if you know what you're doing. I think learning SE is more difficult, but it is more solid in the long run.

SE has developed a specialty around large assemblies. I like SW multibody better. SW surfacing is better, SW training is better, but SE support is MILES ahead of SW. SE support all comes from a central organization GTAC from people who have been there and know what they're talking about. SW support is the lowest rung on the reseller channel ladder, so you're usually talking to someone who has less experience in the software than you do. SE has some really great internal communication tools. SW is less standardized, and you get whatever you get from resellers (who I imagine are kind of annoyed at SW right now).

To me, the biggest difference is between the parent companies. Dassault seems to be annoying a lot of users right now. Siemens is at least less evil. I think Siemens will always give you a way forward, where with DS it's too often a dead end.

If I had to pick right now, for a short term project I'd use SW because I know it better. For a long term project I'd pick SE because the company is more reliable.

[bnemec]

People will only be able to give you their perceptions of the software they have experience with >in the context of how they used it< For example I will be of no use to talk about Solid Edge Sync Tech or Top Down modeling, because we just never used those portions of the software. It might help others to help you if you can explain a bit about how you plan on using the software. Are you doing all one off projects where once the design is released you never see it again? Are you doing skid/platforms with all structural steel sections or consumer goods or packaging or tooling? Do you have a historical data set that is still actively maintained and old parts used in new designs? Matt put together a great response IMO, but you know he wrote a complete book on Solid Edge Sycn Tech alone.

Since we just switched from SE to SW, I wish I would have read the last few lines in Matt's post two years ago. Anyway I thought about your comment of having no experience with Solid Edge. Here's what I suggest, you spend 1-2% of your company's annual design/engineering labor hours in that CAD system doing exactly the kind of stuff you plan on doing. Don't work through canned examples, try to do what you do what you plan on doing for real production usage. See how that goes. Don't assume anything.


Edit: Completely concur with Matt on the tech support on Solid Edge side. A single post cannot convey how awesome the people at GTAC are and how they can advocate for the users to development without traversing many organizational layers like SW has.

[bnemec]

While reading yet another thread about multiple versions of SW installed I was reminded how nice it is to not have to worry about that with Edge. There is no installing two versions. There is a tool for testing another version where you can have another version installed, but it's more just for temporary, testing use.

[bnemec]

Solid Edge still uses separate file type for sheet metal and solid part. It mattered a long time ago it's irrelevant now because they have added function of switching back and forth. IMO, SE is better overall with sheet metal stuff than SW.

I kinda think they should just get rid of the .psm file type. Matt or some other can probably correct me on that though.

[matt]

Solid Edge still uses separate file type for sheet metal and solid part. It mattered a long time ago it's irrelevant now because they have added function of switching back and forth. IMO, SE is better overall with sheet metal stuff than SW.

I kinda think they should just get rid of the .psm file type. Matt or some other can probably correct me on that though.

No, I don't really have an opinion on that, or at least not a good one. I do miss the grab-and-drag flanges. The file types don't bother me one way or the other.

[Jaylin Hochstetler]

Thanks for all of the info guys!

Are you doing all one off projects where once the design is released you never see it again?

We do virtually no one off projects. We are a company that manufactures our own product lines so our files are used for the entire life of the product (which is usually 10+ years) unless of course we have to remodel it for whatever reason. See https://www.dyna-products.com for more info about the machines we manufacture.

Are you doing skid/platforms with all structural steel sections or consumer goods or packaging or tooling?

I would say 50% of our designing is sheet metal, 25% structural, and 25% solid bodies (machined parts, vendor components we model for our final assemblies, & etc.)

[bnemec]

Thanks for all of the info guys!

Are you doing all one off projects where once the design is released you never see it again?

We do virtually no one off projects. We are a company that manufactures our own product lines so our files are used for the entire life of the product (which is usually 10+ years) unless of course we have to remodel it for whatever reason. See https://www.dyna-products.com for more info about the machines we manufacture.

Are you doing skid/platforms with all structural steel sections or consumer goods or packaging or tooling?

I would say 50% of our designing is sheet metal, 25% structural, and 25% solid bodies (machined parts, vendor components we model for our final assemblies, & etc.)

First off, Awesome products!!!! You're welcome to swing by my place any time if you want to test some out!

Before you buy have a plan figured out of how you're going to get the models you need into the new CAD system. We skipped this and it's a regret. Take the time first, you can get demo licenses, use them. Oh, and all our SE models are laying on their faces when imported into SW. SW thinks Y+ is up and Z+ is out front, SE (and the rest of the 3 space world) thinks Z+ is up and Y+ is out back; if you ask me it's because the Solidworks guys kept their drafting boards steeper than 45 degree angle and Unigraphics guys kept their drafting boards closer to horizontal. So if you plan on using dumb imported geometry (valid plan considering sync tech and direct editing tools in SE) you will want a plan to deal with that. I'm assuming your SW models will be laying on their back when imported to SE. We tried all kinds of things to deal with it, the only clean solution was to use direct edit in SE to rotate -90 about X before saving the X-T file. Then it's fine when imported into SW. Again, if we would have taken our time we would have been able to come up with an API to automate this process of rotate, parasolid out, import, fix name, save file, check in to pdm, etc. But we didn't, don't do that.

Just my little bit of experience, don't apply without chewing on it a little first.

[Jaylin Hochstetler]

Thanks for the info @bnemec! It's definitely good to know before we dive into it. We definitely plan on getting a free trial b4 we up and buy it. I think with the free trial we will better be able to tell if it is a fit for us.
We had a demo w/ Siemens (Sean Barry and Kyle Aruda were the demonstrators, they are very helpful guys. Kyle said he's known you @matt for quite some time!) and they imported one of our assemblies w/ the part files and a drawing. The drawing and the part files came through good but it did not recognize the mates in the assy.

[matt]

... Kyle Aruda ... Kyle said he's known you @matt for quite some time!

Kyle was at Siemens when I first got there. Or maybe we met at one of the PLMWorld conventions before I started. Say hi to him if you see him again!

[AlexLachance]

Thanks for the info @bnemec! It's definitely good to know before we dive into it. We definitely plan on getting a free trial b4 we up and buy it. I think with the free trial we will better be able to tell if it is a fit for us.
We had a demo w/ Siemens (Sean Barry and Kyle Aruda were the demonstrators, they are very helpful guys. Kyle said he's known you @matt for quite some time!) and they imported one of our assemblies w/ the part files and a drawing. The drawing and the part files came through good but it did not recognize the mates in the assy.

Has the company or anyone inside the company gone through the process of migrating from a program to another? If not, you should get an advisor, there is a lot of things to take into concideration when doing the switch.

[Jaylin Hochstetler]

Thanks for all of the info guys!

Are you doing all one off projects where once the design is released you never see it again?

We do virtually no one off projects. We are a company that manufactures our own product lines so our files are used for the entire life of the product (which is usually 10+ years) unless of course we have to remodel it for whatever reason. See https://www.dyna-products.com for more info about the machines we manufacture.

Are you doing skid/platforms with all structural steel sections or consumer goods or packaging or tooling?

I would say 50% of our designing is sheet metal, 25% structural, and 25% solid bodies (machined parts, vendor components we model for our final assemblies, & etc.)

First off, Awesome products!!!! You're welcome to swing by my place any time if you want to test some out!

Thanks for the comment @bnemec ! They definitely are awesome machines!
We actually have a dealer in Wisconsin:
West Shore Tool Service
Pestigo, WI, USA

Just in case you're ever interested in one.

[mike miller]

Thanks for all of the info guys!



We do virtually no one off projects. We are a company that manufactures our own product lines so our files are used for the entire life of the product (which is usually 10+ years) unless of course we have to remodel it for whatever reason. See https://www.dyna-products.com for more info about the machines we manufacture.


I would say 50% of our designing is sheet metal, 25% structural, and 25% solid bodies (machined parts, vendor components we model for our final assemblies, & etc.)

First off, Awesome products!!!! You're welcome to swing by my place any time if you want to test some out!

Thanks for the comment @bnemec ! They definitely are awesome machines!
We actually have a dealer in Wisconsin:
West Shore Tool Service
Pestigo, WI, USA

Just in case you're ever interested in one.

Oooooo....spammer.

[Jaylin Hochstetler]

First off, Awesome products!!!! You're welcome to swing by my place any time if you want to test some out!

Thanks for the comment @bnemec ! They definitely are awesome machines!
We actually have a dealer in Wisconsin:
West Shore Tool Service
Pestigo, WI, USA

Just in case you're ever interested in one.

Oooooo....spammer.

Oh, SHUT UP!

[Glenn Schroeder]

I have zero experience with SE, but do have one comment regarding @matt's comparison about service. All VAR's aren't created equal. I've dealt with two of them extensively; GoEngineer and MLC Cad, and have received very good service and tech support from both.

[uk_dave]

I have no proverbial dog in this fight (for obvious reasons) but I do just want to say thank for all the kind words on the quality of support received from PLMS (formerly GTAC). We pride ourselves on our support, really do care, and do try hard to provide a quality experience. Plus, on the Solid Edge side of support, we are a nimble organization that is able to proactively react to and provide fast turnaround with fixes and solutions.

I was a customer, user, and CAD administrator for over twenty years for the majority of the bigger CAD software solutions and having experienced technical support from all of them. I personally ranked GTAC (now PLMS) as one of the best and that was certainly a huge factor in my moving over in to the PLMS world of support.

[matt]

...PLMS (formerly GTAC)...

You know, they never ask me before they change names like this.

Hey, Dave, how you doing?

[bnemec]

I have zero experience with SE, but do have one comment regarding @matt's comparison about service. All VAR's aren't created equal. I've dealt with two of them extensively; GoEngineer and MLC Cad, and have received very good service and tech support from both.

Completely agree Glenn. I can only speak from my experience and my comments about GTAC (now PLMS I see) were not as a negative towards SW VARs. It may be that when something is ranked above others that the others are bumped down the scale; I would say that the way that GTAC can provide support puts them on a different scale. Due to the layering differences I just don't think it's fair (or accurate) to compare what GTAC can provide to the end user vs what VARs can provide to the end user. If we must talk the quality of staff (people) I've had great experiences from both, I just don't see any problem there.

[Jaylin Hochstetler]

Yea, it wouldn't take much to have better service than SW. Though I do agree with @Glenn Schroeder that not all VARs are the same. Our current VAR is GoEngineer and we have had fairly good luck w/ them so far.

[matt]

I have worked for 3 SW vars, and they ALL put noobies on tech support (including me when I first started). It's a great place to learn, but sometimes they learn at other's expense. And eventually they know a lot.

[AlexLachance]

Honestly guys, if your VAR is not giving you adequate service, speak up. Reach out to someone higher then the support guy, and if they can't fix it internally then reach out to someone from SolidWorks.

I've gone through this, had really awful support at first but since I spoke with someone at SolidWorks, everything has gone for the best since. Great, quick and persistent support.

[Ry-guy]

Thanks for the info @bnemec! It's definitely good to know before we dive into it. We definitely plan on getting a free trial b4 we up and buy it. I think with the free trial we will better be able to tell if it is a fit for us.
We had a demo w/ Siemens (Sean Barry and Kyle Aruda were the demonstrators, they are very helpful guys. Kyle said he's known you @matt for quite some time!) and they imported one of our assemblies w/ the part files and a drawing. The drawing and the part files came through good but it did not recognize the mates in the assy.

Has the company or anyone inside the company gone through the process of migrating from a program to another? If not, you should get an advisor, there is a lot of things to take into concideration when doing the switch.

If you are moving from a Parasolid to Parasolid tool..there is not "translation". If you plan to go to STEP and then to the new system then you are in for a challenge. Solid Edge does a greatjob of importing and mapping. You just need to take the time to go through and configure the process!

[Ry-guy]

I know this is a controversial subject, but I'm curious what y'all have to say. We are actively looking into SE and I would love to here some of the pros and cons.

What are some of the pros and cons?
What are some of their good points and bad points?
How do their workflows compare?
What features does SE have that SW doesn't? (to mention some I know of: synchronous technology, dimension tracker in drawings, a built in low end PDM w/ all licenses, you can wait to update your drawings so if a DV loses a reference you can still save the drawing as a rev. before updating, and they offer a better CAM and Illustrator.)
What features does SW have that SE doesn't?
How does their sheet metal design/workflow compare?
How does their weldment design/workflow compare?
How do their assemblies compare?
How does their multibody part design/workflow compare?
How do their drawings compare?

These are a couple of comparisons I could think of, feel free to add to it.
I personally don't have any experience w/ SE but I'm sure some of you others do and can contribute to this.

Pros:
1. The parent company uses this software to develop their own products! That says a lot to me!
2. You are getting software from a company that licneses their technology to their competitors. Says alot about who is a technology leader!
3. Solid Edge software provides more functionalty for a smaller investment than does the competitor.
4. Solid Edge's product development group develops components that are used in the high-end CAD tools. Must be doing something right.
5. The parent company is not trying telling you how to use your software tools.

Cons:
1. Doesn't have a big flashy marketing group promising experiences! They only promise productivity.
2. Provides you the flexibilty to design your products using multiple methods while working with design data. Can make choosing the right tools harder.
3. Requires a user to actually think about design instead of thinking about a design strategy to build a part- that may or may not ever get changed in the future.
4. Requires a user to re-evaluate their old habits and form new ones- like being productive. ;-)
5. Provides a user multiple ways to manage their own data. Decisions, decisions...
6. Require a user to understand that their settings on their workstation will be mapped to their home workstation via the cloud (if you go that route)..You might need to worry if it is sunny outside. No clouds when it is sunny.
7. A user might actually enjoy doing design work and solving business problems instead of solving SW workaround problems. What will you do with your free time!? Maybe sip bourbon or highland scotch?

Oh, Solid Edge comes with sub-d modeling. If you have to make any organic or Class A shapes you will appreciate this tool.
Oh, Solid Edge has bi-directional connectivity to ECAD..honestly it does!
Oh, Solid Edge has a built-in Requirement Management connectivity to Polarion. If you aren't in a regulated environment this might not mean much to you..but if you are... Solid Edge and NX are the only tools that has this connectivity.
Oh, you get Teamcenter Share for collaboration..doesn't sound like much but think about doing your Solid Edge data management functions on the Share site...then you now have cloud-based PDM and collabortaion tools. I still have to verify this will work, though!

What have you gotten from SolidAlmostWorks in the last 5 years? More bugs? Continually ignoring fixing old bugs, icon changes? Maybe a refeshed PDM Pro dialogs? Something to think about.

[SPerman]

Honestly guys, if your VAR is not giving you adequate service, speak up. Reach out to someone higher then the support guy, and if they can't fix it internally then reach out to someone from SolidWorks.

I've gone through this, had really awful support at first but since I spoke with someone at SolidWorks, everything has gone for the best since. Great, quick and persistent support.

If I ever renew my SW license it won't be with my current VAR. They are terrible. Last October I got fed up and ended up on a call with Mike Sabochek along with a few people from the VAR. They were more responsive for a little while, but it didn't last long.

[AlexLachance]

Honestly guys, if your VAR is not giving you adequate service, speak up. Reach out to someone higher then the support guy, and if they can't fix it internally then reach out to someone from SolidWorks.

I've gone through this, had really awful support at first but since I spoke with someone at SolidWorks, everything has gone for the best since. Great, quick and persistent support.

If I ever renew my SW license it won't be with my current VAR. They are terrible. Last October I got fed up and ended up on a call with Mike Sabochek along with a few people from the VAR. They were more responsive for a little while, but it didn't last long.

Speak up Scott. I went through the same process. I complained a lot to my VAR, there was one dude that was more receptive then the rest of them over there. He's now the director of that VAR, but that has nothing to do with me, his hard work and dedication is what brought him there.

But back to the story, I had lodged a lot of tickets and none of them were getting answered so I ended up on the forums and after a little while of complaining about the issue from the time to time, Matthew Lorono contacted me about it and then came over to meet us personally and reassure us that their intent was to have the VAR provide the best service possible and as quickly as it could be.

Since then, the service I have received from my VAR has been top notch, I'd even go to the extent to say flawless, but that would mean that SolidWorks actually did something, so I'll leave it at top notch.

Maybe try speaking to the top brass, or build yourself a ''case'' to display the lack of service.

[SPerman]

Why do I want to invest that much time and energy when I can choose to support a VAR that wants to do it correct without me raising a stink?

If a phone call with Mike Sabochek didn't help, I'm not sure what will. (https://www.linkedin.com/in/msabocheck/)

[mike miller]

Here we go.....

2021-03-23 17_15_24.jpg

[matt]

Here we go.....

2021-03-23 17_15_24.jpg

Have fun!

[DaveG]

Here we go.....

2021-03-23 17_15_24.jpg

Not sure what learning resources are available to you, I found John Devitry's courses on Udemy to be excellent.
https://www.udemy.com/courses/search/?s ... hn+devitry

[Jim Elias]

I think it depends on the environment. If you are often dependent on freelancers/externals, SW is the better bet because the user base is simply an awful lot bigger. The chances you will quickly find someone who knows his/her CAD chops are simply better.

If you are strictly staff-designers, or you're a lone-wolf innovator, you might as well look at everything out there. I know several jobbing-shop owners who saved tons of money going with "smaller-house" systems. They say that the support is fine. But good luck finding anyone on short notice who has the same system, let alone is ready to hit the ground running with it.

I have SW (and NX), have done gigs in SE (and IV and Creo), and I think that there is no general magic-bullet system. When working with something new, there is always something cool compared to what you've known before, whether it's synchronous stuff or better drafting shortcuts or whatever. Then you're still back to the head-sweat.

[Ry-guy]

I think it depends on the environment. If you are often dependent on freelancers/externals, SW is the better bet because the user base is simply an awful lot bigger. The chances you will quickly find someone who knows his/her CAD chops are simply better.

If you are strictly staff-designers, or you're a lone-wolf innovator, you might as well look at everything out there. I know several jobbing-shop owners who saved tons of money going with "smaller-house" systems. They say that the support is fine. But good luck finding anyone on short notice who has the same system, let alone is ready to hit the ground running with it.

I have SW (and NX), have done gigs in SE (and IV and Creo), and I think that there is no general magic-bullet system. When working with something new, there is always something cool compared to what you've known before, whether it's synchronous stuff or better drafting shortcuts or whatever. Then you're still back to the head-sweat.

OK. I have a beef with this line of thought. As a business owner why am I giving away my data in formats that my customer can then take and make all the design changes on? Design changes is were the business makes money. The organizations I've worked for have had policies where they require a 3D model and pdf. Not native CAD data. If a customer is requiring you to supply native CAD data then you should be charging a premium. It's your business to be efficient with your design tools. That's where I think SE shines. Making changes super fast and super easy. Even to the point of making changes to multiple parts in an assy at one time.

[jcapriotti]

@Ry-guy In my experience, whenever we hired an outside company to design something for us due to lack of internal resources or knowledge, we own the data and files. They must be in our format and compatible version. I suppose it would be different if you own the product and only "tweaked" if for a specific customer, we buy those designs as well. That vendor still gives us native SolidWorks files (if they use SolidWorks) but we would be in violation if we were to make the design ourselves.

[Rob]

A few years ago there was an amazing deal for Solid Edge. If you had a SW license they would basically give you a free SE license - all you had to do was buy 3 years subs.

Anyway I took a free trial but unfortunately my PC kept getting BSD (blue screened). When I uninstalled SE this fixed the problem, but unfortunately it put the brakes on me giving SE a proper assessment.

I'm now considering looking at SE again. We would have to run both systems.

Has anyone else had problems running both SE & SW on the same machine? - it was a while ago on Win 7.

I never got to the bottom of it and work commitments forced my hand to cease the trial prematurely.

[bnemec]

A few years ago there was an amazing deal for Solid Edge. If you had a SW license they would basically give you a free SE license - all you had to do was buy 3 years subs.

Anyway I took a free trial but unfortunately my PC kept getting BSD (blue screened). When I uninstalled SE this fixed the problem, but unfortunately it put the brakes on me giving SE a proper assessment.

I'm now considering looking at SE again. We would have to run both systems.

Has anyone else had problems running both SE & SW on the same machine? - it was a while ago on Win 7.

I never got to the bottom of it and work commitments forced my hand to cease the trial prematurely.

Hi Rob.
We have been running SE2019 and SW2019SP4 on all our CAD machines since November 2019. The only problem we know of was PDM using some solid edge dll for preview tab and that caused bad UI performance in Solidworks. We have no intention to keep using both, trying to get all the models into Solidworks is taking much longer than expected.

[Jim Elias]

OK. I have a beef with this line of thought. As a business owner why am I giving away my data in formats that my customer can then take and make all the design changes on? Design changes is were the business makes money. The organizations I've worked for have had policies where they require a 3D model and pdf. Not native CAD data. If a customer is requiring you to supply native CAD data then you should be charging a premium. It's your business to be efficient with your design tools. That's where I think SE shines. Making changes super fast and super easy. Even to the point of making changes to multiple parts in an assy at one time.

Probably depends on the market... in my industry, design changes after production release are usually unprofitable distractions. The earning is done on developing the product.

@Ry-guy In my experience, whenever we hired an outside company to design something for us due to lack of internal resources or knowledge, we own the data and files. They must be in our format and compatible version.

So say my clients as well. They want native model, live drawing file, PDF drawing snapshot, and usually a STEP model snapshot.

[jcapriotti]

So say my clients as well. They want native model, live drawing file, PDF drawing snapshot, and usually a STEP model snapshot.

Ironically, the only time we didn't own the data after development of a component was internal at an overseas division of our own company. They wanted to own the design, development, and manufacturing for 3 years after which it was turned over to our division. Ah, internal politics......

[mattpeneguy]

A few years ago there was an amazing deal for Solid Edge. If you had a SW license they would basically give you a free SE license - all you had to do was buy 3 years subs.

Anyway I took a free trial but unfortunately my PC kept getting BSD (blue screened). When I uninstalled SE this fixed the problem, but unfortunately it put the brakes on me giving SE a proper assessment.

I'm now considering looking at SE again. We would have to run both systems.

Has anyone else had problems running both SE & SW on the same machine? - it was a while ago on Win 7.

I never got to the bottom of it and work commitments forced my hand to cease the trial prematurely.

Rob,
I'm still running windows 7 and demoed SE a while back. I didn't have any problems with it, but couldn't fully evaluate it, even though they extended my trial period.
Nothing stood out that seemed to prevent us from moving over. And I've read it's easier to get SW files into SE than vice versa.
SE did some things better, their mouse gestures are much better. Their drawing views were much better with clipping, just working better. You could search for a SW term and the SE equivalent would show up. A good bit more of the animated tool tips showing how to use the tools were there. Using it made me think that Seimens was actively trying to make it easier to transition.
Unfortunately just like SW it's complicated and I didn't get into things like how their custom properties work.

[Melo]

Personally I can't compare as I never used Solidworks. I'm a Solid Edge user. But my colleague worked with Solidworks for a few years until version SW 2016 and the main difference he point out when compared to Solid Edge is stability. He said that a crash in Solidworks was "just another day at the office" as it happened frequently, and when he moved to Solid Edge he had his first crash after 6 months, so this is something he points out: stability.

[SPerman]

How does SE handle arrangements/configurations? It looks like they call it "alternate assemblies" but I would like to hear from SE users how well this works, and how it compares to NX arrangements/SW configurations.

https://docs.plm.automation.siemens.com ... masm1a.htm

[bnemec]

How does SE handle arrangements/configurations? It looks like they call it "alternate assemblies" but I would like to hear from SE users how well this works, and how it compares to NX arrangements/SW configurations.

https://docs.plm.automation.siemens.com ... masm1a.htm

The company I work for used SE for about 20 years, many of the early files are still in used and maintained. We didn't use FOA, they were troublesome in our use case. I don't recall all the details and several of the failed attempts were before my time here. One thing I remember vividly is if you have a FOA, then have a drawing (draft) and double click a view to open the assembly, SE would open up to the family member that was used in the drawing view you double clicked on. Then if you saved the assembly file you would loose access to all the other family members. We had some calls with GTAC over that, solution was to stop using FOA again.
Again, I wish there were some from the SE forum over here now and again to add more perspectives and experience as I can only share what I encountered.

[Ry-guy]

How does SE handle arrangements/configurations? It looks like they call it "alternate assemblies" but I would like to hear from SE users how well this works, and how it compares to NX arrangements/SW configurations.

https://docs.plm.automation.siemens.com ... masm1a.htm

You can't compare NX Arrangements with SW configurations. They serve different functions. NX Arrangements is a display tool that allows you to "reposition" and hide/show assembly components. You can actually build steps that allow you timelines and even assembly sequencing of a product.

SW Configurations is primarily used as a product/design configuration tool. Where you manage design elements in a table.

Solid Edge alternate Assemblies work very much like SW configuration. Here you can control existing component locations/postitions and/or you can have different component parts. SW and SE are close enough to each other that Solid Edge uses the SW API to actually migrate SW configurations into Solid Edge alternate assemblies.

[Ry-guy]

How does SE handle arrangements/configurations? It looks like they call it "alternate assemblies" but I would like to hear from SE users how well this works, and how it compares to NX arrangements/SW configurations.

https://docs.plm.automation.siemens.com ... masm1a.htm

The company I work for used SE for about 20 years, many of the early files are still in used and maintained. We didn't use FOA, they were troublesome in our use case. I don't recall all the details and several of the failed attempts were before my time here. One thing I remember vividly is if you have a FOA, then have a drawing (draft) and double click a view to open the assembly, SE would open up to the family member that was used in the drawing view you double clicked on. Then if you saved the assembly file you would loose access to all the other family members. We had some calls with GTAC over that, solution was to stop using FOA again.
Again, I wish there were some from the SE forum over here now and again to add more perspectives and experience as I can only share what I encountered.

Families of Assemblies and family of parts was striclty a legacy CAD function to quickly generate similar designs and assemblies. These functions are great when you are not dealing with a PDM or PLM. When you start operating in managed environments these type of tools become a huge encomberance. The PDM tool wants to do its job and managed the data and boms. That really conflicts with the concept of FOAs and part families- where the top level assembly wants to control the files!

[Jaylin Hochstetler]

I was experimenting with SE the other day and was really pleased w/ what I saw regarding drawings, BOM mating, and automated exploded views.
Attached is a video I took where I mate a couple parts, make an exploded view, make a drawing w/ an exploded view, BOM, and balloons.

[Roasted By John]

What about "Custom Properties"????

[Jaylin Hochstetler]

What about "Custom Properties"????

Haven't messed w/ em much but this is what the window looks like:

And here it is in a drawing:

Sadly they don't have a property tab builder.

[Ry-guy]

Haven't messed w/ em much but this is what the window looks like:
image.png
And here it is in a drawing:
image.png
Sadly they don't have a property tab builder.

See if this works...I am working from memory and at 50 it's getting sketchy!

No, Solid Edge is not in the business of creating a bazillion custom properties for files. Those type of tasks belong to an PDM (if you didnt' know you have a built-in PDM tool when you use Solid Edge!!) or PLM tool!

So, as I recall there is a seed file for custom properies..seedprop.txt or propseed.txt something like that..sorry don't have to google that, today. Take a look at that...then take a look at the videos for Solid Edge Bulit-in Data Management..you might be happily surprised!

[Imics13]

Haven't messed w/ em much but this is what the window looks like:
image.png
And here it is in a drawing:
image.png
Sadly they don't have a property tab builder.

Hi,

I suggest using Property Manager from Data Management Tab. It's very similar to PB, you can customize it (RMB on a cell).

BR,

[bnemec]

We are really missing the "Dimple" features in Solid Edge. In Solidworks, there is no dimple from sketch, it requires another part file "forming tool". The fact that the references from the sheet metal part file to the forming tool file is not made in PDM is just salt in the wound.

[jcapriotti]

I think the SWX thought behind it is that forming tools are custom with set dimensions, so you build a "tool" library. They are configurable for several sizes.

You can put the tools in a PDM library folder set to "cache". That's what we do. I just wish there was a way to tell PDM to force clients to cache on a state change so when we update a library cut or forming tool, it updates each client.

[bnemec]

I think the SWX thought behind it is that forming tools are custom with set dimensions, so you build a "tool" library. They are configurable for several sizes.

You can put the tools in a PDM library folder set to "cache". That's what we do. I just wish there was a way to tell PDM to force clients to cache on a state change so when we update a library cut or forming tool, it updates each client.

I think you are right, that sounds similar to what I've been told by others concerning forming tools. That may be nice for some but over ~90% of our forming tools are only used on one part. So there is no gain by having another file. Maybe we're one in a thousand that have no need to reuse forming tools, I don't know. I do know that a dimple or bead from a sketch is much simpler to create and maintain than using another part file for the task.

We do have the forming tool files in the vault. Similar to you we wish PDM would resolve the reference from the part to the forming tool. The forming tools are in a location that is updated on login, so we're usually ok there. The problem is I've been harping on users to check files in when they're not working on them, per "best practice" advice I've received, but those forming tools do not show up in the Ref File Dialog when the user is checking the part file in or out. Then they forget that they need to manually check the forming tool file out/in. So there's been a bit of not able to save the forming tool because it was not checked out when they edited it.
It feels like this is one of those gaps that are left behind when a company buys some other system and invests just enough to get it integrated for demos or ~80% of the users, but not enough to get all the areas where the two affect each other smoothed out.