synchronous technology

[matt]

Is Siemens spelling synchronous technology with capitals or lower case these days? I could never keep that straight.

Anyway, I wanted to get SE users opinions on ST. Do you use it? Have you tried it? What kind of parts do you make?

I wrote an ebook for ST while I was there that never really got distributed properly. It was called "Synchronous For History Based Users", and it made the case for using sync instead of or in conjunction with some history-based features. It's a 320mb download. 10 pdf chapters with sample models. It might be a little dated by now (probably 5 years old).

I have spent a lot of time messing with the history tree, fixing, repairing, etc etc stuff that never should have broken. So I got tired of history based software, and started looking into direct edit type stuff. For certain types of models, synchronous is really a great tool. The ebook addresses most history-based users arguments against sync. It was written from a technical perspective (but funded by the marketing department).

If you're a skeptic, you owe it to yourself to check it out. http://dezignstuff.com/STFTHBU/STFTHBU.zip

[ChrisM_Oneplm]

Always love to see stuff about Synchronous. It has its place.

https://youtu.be/jcUMppKftn4

[bnemec]

Matt, you were one of the ST pushers that kept me looking at it again and again. We could never get over the lack of fixing the geometry. I don't know that I ever fully understood the "design intent" rules or what they were called. I can see it being indispensable for some use cases. We couldn't figure out how to contain it and control it in our use case.

Again, possibly due to my lack of ability to grasp how the design rules worked. We have a bunch of users that would have needed trained and more than just a one day course, that was tried.

[matt]

Matt, you were one of the ST pushers that kept me looking at it again and again. We could never get over the lack of fixing the geometry. I don't know that I ever fully understood the "design intent" rules or what they were called. I can see it being indispensable for some use cases. We couldn't figure out how to contain it and control it in our use case.

Again, possibly due to my lack of ability to grasp how the design rules worked. We have a bunch of users that would have needed trained and more than just a one day course, that was tried.

Yeah, it's a different way of looking at CAD. Mostly if you think of the live rules or design intent as being like sketch relations for the 3D solid, that was the big concept. The feature was whatever faces you select, and stuff doesn't move unless you tell it to. I think some of the training material tried to force people to get too fancy too fast. Once you get comfortable with the simple concepts, the more complex moves become easier to control.

[jcapriotti]

Wish I could try it, but after watching video after video it looked like a steep learning curve for the more casual CAD user. Obvious you are not the average CAD user @matt.

History base seems like it would be easier to see what's going on in more complex models as its broken into the manageable pieces of sketches and features. 3D constraints feels like it could get overwhelming quick. Kind of how we tell new user's not too put too much in single sketch. Too many sketch relations solving at the same time can cause issues and its harder to troubleshoot when things go wrong.

I'm sure I'm missing something having not had the chance to try it out.

[Jaylin Hochstetler]

We are checking into SE and have a couple questions someone might be able to answer.

• How does SE handle multibody parts? From what I here it is more assembly oriented, is that correct? Currently we put everything that is welded in one MB part. And then everything else is put in the assembly. Then we use cutlist properties to pull weldment and sheetmetal data. I read this https://community.sw.siemens.com/s/ques ... -some-love post and wasn't quite sure what to think.

• Does SE have something similar to SW cutlist properties, or is it intended to use all individual parts?

• In your experience, is it worth the pain of migration for the benefits of synchronous technology? I have seen some videos and sat in a demo of synchronous technology and was very impressed.

Any info is much appreciated.
Thanks in advance!

[matt]

@Jaylin Hochstetler I don't really know much about the weldments in SE. I did work with the multibodies, and it is different from SW's implementation. In SE, you can have a single body that is made up of multiple volumes. I think the terminology they used was "lumps". You can have multiple lumps/volumes within a single body, until you tell it that you're now working on a new body. I personally didn't get it. I was there when they did this. They did ask me a lot of questions before they implemented multibody, but I had a really hard time working with whatever they came up with. I was focused on surfacing and synchronous.

My experience with multi-bodies and assemblies, even in SW, is don't try to use one when you should use the other, and don't get hung up on multibodies instead of assemblies. Work the way the software was meant to work. If you try to argue with the software, you'll lose every time.

Synchronous is great, especially for imported parts, and especially for prismatic parts. Works is comparatively useless for imported data. Imported parts in synchronous SE can work like native data. HUGE difference. You won't believe it the first time you edit an imported part, and you can change fillet radii.

[Jaylin Hochstetler]

Thanks for the info @matt!

The more I research into SE the more I discover SE is more geared toward assemblies, rather than MB parts.

[bnemec]

You can do Multi body in SE, they have mold/tooling features of split and save out to separate files. They had the usual boolean operations, which I really like when things get complicated. I cannot speak to the weldments and cutlists as we always had one part number per file. As Matt mentioned they started allowing bodies to have disconnected solids just a few years ago. Multi body was clunky compared to my experience in IV or SW; in SE you must start a new body then start the feature, in the other two you can tell the feature to merge or make new body.

As far as converting, how many of your old files do you need to use going forward? percentage.

[Jaylin Hochstetler]

As far as converting, how many of your old files do you need to use going forward? percentage.

I would say we would probably have to convert around 80% of our files that are currently in use. We have a lot of really old files we no longer use that we would not have to convert. The other 20% of our current in use files we would probably remodel so we can keep our workflow more consistent. .Then again I don't have any experience w/ SE so I'm not sure how many of our files we would have to convert.
We are a manufacturing facility that manufactures our own product line so we use our files for the life of the product which can be quite a number of years. (I'm always jealous of the guys who get to work with one time parts that have a short lifetime) A couple of years ago the engineer prior to me completely redid most of the files b/c the engineer prior to him didn't know what he was doing and really screwed things up. And we don't like the workflow the previous engineer used (he used the horrible horrendous saved bodies) so we would probably redo quite a bit of the files in order to keep the workflow consistent.

What workflow works best in SE, top down, multi-body?

[matt]

It's hard to answer anything without knowing what kind of stuff you're doing. But I'll just assume your parts don't use lofts or complex shapes. If most of your features are extrudes, and you don't use splines, then SE will work well for you as long as you can embrace the synchronous technology way of working. ST is essentially direct edit with some brains behind it. It can make changes to imported parts and recognize things like patterns to change them. Feature order is non-existent, and you can change whatever you select. You put dimensions and relations directly on the 3d model, kind of like you do on sketches in SW. Of course SE also allows you to work in history-based mode. And it has subd mode as well. SE can work top down or multibody, but I think the smart money is on synchronous assemblies. All the power of history-based top down (and then some) without the best practice headaches.

[SPerman]

I guess I haven't seen the right synchronous technology tutorial yet. All the videos I see show you being able to drag stuff around, but if there aren't dimensions associated with it I don't see the value. I know I'm not the only one who needs parts to precise dimensions, so there must be more to it than what I've seen in videos.

[mike miller]

I guess I haven't seen the right synchronous technology tutorial yet. All the videos I see show you being able to drag stuff around, but if there aren't dimensions associated with it I don't see the value. I know I'm not the only one who needs parts to precise dimensions, so there must be more to it than what I've seen in videos.

Check this one out. https://solidedge.siemens.com/en/resour ... n-changes/

[matt]

I guess I haven't seen the right synchronous technology tutorial yet. All the videos I see show you being able to drag stuff around, but if there aren't dimensions associated with it I don't see the value. I know I'm not the only one who needs parts to precise dimensions, so there must be more to it than what I've seen in videos.

Yeah, I'm not sure the people writing the demos are doing the right thing. Essentially treat a 3D solid part like a sketch, except if you don't dimension it, give it a relation, or tell it to move, it will stay where it is. So you can put dimensions on a box with a hole on it, and make changes to it. The changes can be visual (dragging it around) or dimensional. You can also have it automatically select things based on rules. This is the thing they demo, and this is the thing that scares people. You don't have to use those auto-select rules until you get comfortable with the system.

It's really cool, fully parametric. It's not magic, You have to let go of some of your fears, but using it is liberating. The "feature" is whatever you select. You can make changes with sync that you would never imagine making with history-based stuff.

[SPerman]

That doesn't make me any more excited about the technology.

My take:

The history based model wasn't created with proper design intent. So if you change a dimension bad things happen downstream. (This isn't the fault of history based modelling. And I think this was done intentionally to show how "great" ST is.)

The example using ST doesn't have any design intent. So if you move one face nothing follows.

I've spent the last 20 years using the old school method, so I clearly have lots of bias. But nothing I've seen to date convinces me ST is better, just a different approach.

[mike miller]

That doesn't make me any more excited about the technology.

My take:

The history based model wasn't created with proper design intent. So if you change a dimension bad things happen downstream. (This isn't the fault of history based modelling. And I think this was done intentionally to show how "great" ST is.)

The example using ST doesn't have any design intent. So if you move one face nothing follows.

I've spent the last 20 years using the old school method, so I clearly have lots of bias. But nothing I've seen to date convinces me ST is better, just a different approach.

This video is where the light came on for me. https://solidedge.siemens.com/en/resour ... al-design/

They do things to that model that would be very difficult if not impossible with SWX.

[Ry-guy]

@matt It is just lowercase for both "synchronous technology".

[Jaylin Hochstetler]

This video is where the light came on for me. https://solidedge.siemens.com/en/resour ... al-design/

That video still amazes me after seeing it for the 2nd time.

[matt]

That doesn't make me any more excited about the technology.

My take:

The history based model wasn't created with proper design intent. So if you change a dimension bad things happen downstream. (This isn't the fault of history based modelling. And I think this was done intentionally to show how "great" ST is.)

The example using ST doesn't have any design intent. So if you move one face nothing follows.

I've spent the last 20 years using the old school method, so I clearly have lots of bias. But nothing I've seen to date convinces me ST is better, just a different approach.

I spent 2 years making fun of it too. I've spent so much time pulling my hair out reordering features, going back and fixing broken relations that anything that got rid of that was beautiful. I've spent as much (or more) time in the history-based world. You can make edits to a finished part without caring which faces are part of the base feature.

Demos and demo jockeys are lame. You have to see past that to see what it can really do for you. You could import SW parts and work with them faster than the SW user with native history tree could, and without rolling back the tree to see which features were made how.

Anyway, it's worth having an open mind about.

[Ry-guy]

• Does SE have something similar to SW cutlist properties, or is it intended to use all individual parts?

• In your experience, is it worth the pain of migration for the benefits of synchronous technology? I have seen some videos and sat in a demo of synchronous technology and was very impressed.

You can use Solid Edge Weldments just like SolidWorks. I'm not up-to-date on the new multi-body stuff for things like imported data.

There really isn't a "migration" in the old-school sense. Solid Edge has a very effeictive tool that makes the data and drawing migration pretty straight forward. Simply put, Siemens is using the SolidWorks API tools to map all your drawing elements and element locations to equivalent Solid Edge drawing elements. As for the models, you are going Parasolid to Parasolid so you are not doing any translation. You will lose any intelligence (aka parameters) in your model. But you can also map your drawing dimension to "driving dimenesions" that are converted to PMI and drive you model that way. To me that is more design intent than any history-base plus parameters ever was.
As for assembllies, once again assembly positioning and configurations map over to Solid Edge...so does the material properties!

You gain when moving to Solid Edge. You gain history-free modeling (I know this is a mind bender for most of us), history-based modeling, hybrid modeling (a model that uses both history and history-free elements), convergent modeling (scanned data and b-rep), synchronous technology, generative modeling (getting something that you can actually use!) and a partner, Siemens, that builds all the core technologies that the other CAD players are using to build their tools! Why buy from the middle man? ;-)

Ryan

[SPerman]

If I ever get the opportunity I definitely will.

I would love to see that same demo with a real part. I'm sure it would be slower if he actually cared about more than one dimension. But I also have no doubt it is still significantly faster for a part like that than history based modeling.

The good news about SE is that I can be a grumpy old man if I don't want to adopt the new technology.

[SPerman]

How would a SSP process work with synchronous technology?

[Ry-guy]

Matt, you were one of the ST pushers that kept me looking at it again and again. We could never get over the lack of fixing the geometry. I don't know that I ever fully understood the "design intent" rules or what they were called. I can see it being indispensable for some use cases. We couldn't figure out how to contain it and control it in our use case.

Again, possibly due to my lack of ability to grasp how the design rules worked. We have a bunch of users that would have needed trained and more than just a one day course, that was tried.

Yeah, it's a different way of looking at CAD. Mostly if you think of the live rules or design intent as being like sketch relations for the 3D solid, that was the big concept. The feature was whatever faces you select, and stuff doesn't move unless you tell it to. I think some of the training material tried to force people to get too fancy too fast. Once you get comfortable with the simple concepts, the more complex moves become easier to control.

Well, this is why I like Solid Edge. This is a Creo 2.0 (2013) part that was brought into Solid Edge. You will see that we have history-free features (aka procedural features). That help defined part of the geometry. Then I took a dxf of the Creo drawing and had Solid Edge link those to the 3D model to drive the part! You will see some extra geometry hanging around...that's from the Creo drawing.
Now I have full control of this part and better control than I did in Creo.
Here's a link that bypasses filling out a form. Watch the full thing or move out 14:00 mark and watch from that point.
https://videos.mentor-cdn.com/mgc/video ... -video.mp4

image.png

[Ry-guy]

rather than MB parts.

Sorry, what is MB parts?

[SPerman]

It sounds like SE does SW better than SW.

How does support work with Siemens? When I was using NX we had an in house guy we sent everything through most of the time. But the few times submitted a problem they were always responsive. I think we dealt directly with siemens, but there may have been a VAR involved.

[SPerman]

There is a workflow in SW (and I assume IV) where you have one part with multiple bodies (MB). I don't get it, but lots of people use it.

[Ry-guy]

How would a SSP process work with synchronous technology?

What's SSP?

[Ry-guy]

It sounds like SE does SW better than SW.

How does support work with Siemens? When I was using NX we had an in house guy we sent everything through most of the time. But the few times submitted a problem they were always responsive. I think we dealt directly with siemens, but there may have been a VAR involved.

Support depends..Solid Edge is usually sold through a VAR. So, you would/should go to the VAR first. I say that because when I was working the VAR Channel a VAR was penalized if their customers where by-passing them and contacting Siemens directly for support.

Siemens still has their 1-800 GTAC support system too.

I will say that from a Solid Edge side of the business, support and develope is VERY responsive to their customers. I've seen questions come up on the Siemens Community site for SE where you have the VP of Product Development/Strategy answer technical questions.

NX is a bit different. Their customer base is more complex and the solutions are tied together. Changes in that system take a bit longer to resolve because the impact assessment is soo much greater.

[SPerman]

That is a link to a post describing a top down workflow using a Skeleton Sketch Part.

viewtopic.php?f=3&t=32&sid=2731ea64096f ... dd06d229a3

[Jaylin Hochstetler]

rather than MB parts.

Sorry, what is MB parts?

Here is a good example of a multi-body (MB) part. It has weldments and sheetmetal all in the same part file. We use this for everything that is welded on the machine and then the rest of the parts are put on in the assembly. In my mind if your using SW it's the only way to though I know some guys would disagree with me.

2021-03-18 07_32_38-Window.jpg

[bnemec]

It sounds like SE does SW better than SW.

How does support work with Siemens? When I was using NX we had an in house guy we sent everything through most of the time. But the few times submitted a problem they were always responsive. I think we dealt directly with siemens, but there may have been a VAR involved.

Support depends..Solid Edge is usually sold through a VAR. So, you would/should go to the VAR first. I say that because when I was working the VAR Channel a VAR was penalized if their customers where by-passing them and contacting Siemens directly for support.

Siemens still has their 1-800 GTAC support system too.

I will say that from a Solid Edge side of the business, support and develope is VERY responsive to their customers. I've seen questions come up on the Siemens Community site for SE where you have the VP of Product Development/Strategy answer technical questions.

NX is a bit different. Their customer base is more complex and the solutions are tied together. Changes in that system take a bit longer to resolve because the impact assessment is soo much greater.

That reminds me, we did have a Solid Edge VAR, but I forget about them. They were not much help.

[jcapriotti]

Here is a good example of a multi-body (MB) part. It has weldments and sheetmetal all in the same part file. We use this for everything that is welded on the machine and then the rest of the parts are put on in the assembly. In my mind if your using SW it's the only way to though I know some guys would disagree with me.

That one hurts my well entrenched (and possibly outdated) modeling sensibilities. My brain is screaming "no, that's an assembly". I get why though. I've wanted to use weldments some but we never had much of a case that fit. For your assembly, I think I would've mixed it some and did the weldment base structure as a part then built an assembly with it added the sheet metal parts.

[Jaylin Hochstetler]

Here is a good example of a multi-body (MB) part. It has weldments and sheetmetal all in the same part file. We use this for everything that is welded on the machine and then the rest of the parts are put on in the assembly. In my mind if your using SW it's the only way to though I know some guys would disagree with me.

That one hurts my well entrenched (and possibly outdated) modeling sensibilities. My brain is screaming "no, that's an assembly". I get why though. I've wanted to use weldments some but we never had much of a case that fit. For your assembly, I think I would've mixed it some and did the weldment base structure as a part then built an assembly with it added the sheet metal parts.

We've done it like that, too. But MB parts results in less files. etc.
It can be a pain though if the cutlist properties don't work right. Check out https://forum.solidworks.com/thread/246171 for more details.

[SPerman]

I'm with jcapriotti. That's an assembly. Who cares how many files it is? You manufacture each piece and weld them together.

[jcapriotti]

We've done it like that, too. But MB parts results in less files. etc.
It can be a pain though if the cutlist properties don't work right. Check out https://forum.solidworks.com/thread/246171 for more details.

Yeah, more files I don't much care about, it's more files to manage but we have a system for it that we've used forever. My concern with MB sheet metal is that each of those sheet metal parts need to be sheared, punched/laser, and formed. Then apply custom properties and detailed on a drawing, and it just seems like a nightmare managing several in one model file, I know you can hide everything except the part you want for drawings, but I would think rebuilds would be much longer. Doesn't that huge MB part file get slow with that many features?

[Jaylin Hochstetler]

We've done it like that, too. But MB parts results in less files. etc.
It can be a pain though if the cutlist properties don't work right. Check out https://forum.solidworks.com/thread/246171 for more details.

Doesn't that huge MB part file get slow with that many features?

It's not too bad.
It takes about 25 sec. to do a force rebuild in that MB part and an assy about the same size took about 3 secs.
IMO it's easier to design with design intent in a MB part than in an assy. Then again that's what I am used to.

[mike miller]

With the right tools, multi-body modeling is very stable and fast. It is way more stable than in-context assy modeling, for sure. It is not as change friendly as SSP, but it is easier to understand and manage.

"The right tools" include:

-Display/delete relations
-Parent/child visualization in the tree
-Edit sketch plane