Building the Punch Holder

Well, for what it’s worth, I rebuilt the punch holder in Solid Edge ordered ST4. It was good to do something with more than just a few features in it.


In the course of building this in Solid Edge, I also fixed a few of the more glaring errors in the SolidWorks part. There were some features that seemed duplicated, although I’m sure they had a purpose. For the sake of modeling, though, I removed them. There were only a handful of features that were removed, and I also removed all out of context (interpart) relations. It sped up the rebuild from 41.5 to 37 seconds.

When I completed the part (there are a handful of missing slots and some missing small fillets), I right clicked on the top feature and selected Recompute. I’m not sure what this does exactly, but the time for it to complete was 16 minutes. The only thing I can think of that would cause that is if SE has some sort of equivalent of Verification On Rebuild. (VOR in SW tests every model face against every other model face instead of just testing against adjacent faces). So I made a test. I made a part that should fail if SE is calculating the VOR equivalent. Well, it doesn’t fail. So it’s not using some VOR equivalent, and it still gets a Recompute time of about 16 minutes. Just for comparison, SW can also create this impossible part if you turn off VOR, but if VOR is on, the fillets fail.

In this part, a block is shelled, and then big fillets placed on one end, causing the fillet to break into the shell, which would be impossible in real world parts

I don’t know exactly what that Recompute thing does, but 16 minutes vs 37 seconds isn’t good news. Notice that all of the hoopla about speed is not about the ordered side of Solid Edge. In all fairness, the experience of working in SE was not what I would call slow. The Recompute thing is certainly slow, but the day to day type of work that you would use this for, even with a pattern with nearly 1000 holes in it, was not as bad as you might expect.

The edited SolidWorks part is 22 mb and SE is 37. That’s a big change from the synchronous (imported) part in SE, which was 12 mb. This comparison really should have been between Synchronous and Ordered.

You can download all of these parts here: edited SW2012 punch holder , SE ST4 Ordered punch holder , SE impossible part  .

After getting a deeper look at the model and the ordered side of Solid Edge, I’ve definitely formed some opinions. First, the original SW model was made for manufacturing, and probably a wire EDM process, if I had to guess. There are a lot of holes that are later cut out – so a small hole is gobbled up by a bigger hole. Plus, there are a lot of out-of-context references, which is never a good thing. As a SolidWorks CAD model, this is a poor example. And if I were looking for a model that rebuilt remarkably slowly given what’s in it, I couldn’t have found a better example. This is nothing against Anna. The model was made for a specific purpose, and by using it as a benchmark, it is well outside of that purpose.

Secondly, I have to admit, it’s taking some time to warm up to Solid Edge’s ordered mode. It has a definite workflow that you have to follow. Once you get in the groove with that workflow, you get used to it.

For example, to create a cut:

  1. click the Cut icon
  2. select a sketch plane
  3. draw the cut sketch
  4. click the Ok button for sketch
  5. set the direction of the cut
  6. click Finish
  7. click Cancel to prevent SE from starting another feature

To make a linear pattern (and this one cost me some time to figure out):

  1. create your feature
  2. click the icon for pattern
  3. select the feature to pattern
  4. click on a sketch plane
  5. sketch a rectangle ?!?!wtf
  6. Interpret a series of unlabeled boxes and if you only want a linear pattern, you have to put 1 in one of the boxes

It turns out that the SE patterns have a lot of flexibility, but the interface is inscrutable. I would love to have an unlabeled interface in SW, because maybe they could finally get it out of my way. But when you’re trying to learn something, an unlabeled interface is the kiss of death. You really do have to memorize the SE interface in order to use it. This is its greatest strength (for existing users) and its greatest weakness (for new users). All they need here is an option to have a verbose or sparse interface. I can see that they’ve tried to funnel the user into the workflow, but there’s just not enough user feedback for a beginner to just pick it up and use it.

Above is the command bar that comes up when you punch the Pattern button. It is laying out the overall workflow in the order in which you need to execute commands.

  1. Pattern
  2. Feature
  3. Sketch Plane
  4. Sketch (and inscrutable option stack – why are these options inside the sketch step, and why are we sketching to create a feature pattern anyway???)

That’s the basic workflow alright, but wtf with the sketch? And most of all, after I click Finish, why do I have to click Cancel again to prevent the cycle from repeating itself? When you’ve got an interface this sparse, an unnecessary step sticks out like a sore thumb. Maybe there’s an option to control that.

So in the end, I can see why Solid Edge added Synchronous Technology. The ordered (history based) side of the software is nothing to write home about. If they were going to compete, they needed to rewrite the rules. Synchronous Technology is in some ways simpler, but in other ways gives you a lot of control. The fact that you can still fall back on history-based techniques for those areas of parts that benefit  from that is a big bonus.

I didn’t set out writing this post trying to make ordered look bad, I just wanted to compare. The main point to me is that there is no reason to model this part in a history based scheme. Synchronous fits this part much better, aside from possibly the patterns. The fact that SE doesn’t look great doing it isn’t surprising. What would be real fun would be to test this part with mixing methods – synchronous features, but ordered patterns, mainly to compare the function of procedural synch tech features with the history based feature definitions.  There may also be some explanations for some of the issues mentioned here. One question I have is if building a part in Synchronous mode produces the same result as building a part in ordered mode, then making it Synchronous?

48 Comments

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  1. Does SE do patterned sketch entities well? Maybe a complicated sketch with many holes will produce geometry more efficiently.

    1. No there is no provision (In Sync) to pattern a sketch. The whole purpose of the pattern is to pattern a feature (a hole or slot or something synch tech sees as a feature).

    2. Rick, I think ordered has a method for patterning sketches, but not synchronous. The whole thing in synchronous is to detach the 3d from the sketch.

  2. Perhaps a beginners mode would add a single line of text under the command bar with some hints/clues/description, while a say green outline moves from icon to icon to highlight the next step?

    1. Then again perhaps its just that its a handicap to be fluent in something else and be confronted with learning to do things differently and seemingly oddly at times. Perhaps complete beginners would not be bothered as much and pick up the UI more easily/intuitively.

    2. Neil (and Matt),

      In SE, if you have the PromptBar on the bottom of the screen, it will show information so you know exactly what it is expecting you to do in the current step of a command. I found this to be a great help when taking my first steps in SE.

      1. Carlos, yeah, I should have mentioned the prompt bar. I keep hoping for that in SW, and now SE has it and I ignore it. The times when I did look at it, it was helpful.

        1. Perhaps if it had the option of appearing immediately under the command bar it would be more useful for real newbies. Looking up and down the screen is a bit of a hassle IMO.

          1. OK then but I’m not giving up on it ;) How about asking on install if you want the initial UI to generally resemble Autocad or Solidworks or__? Then Matt can have his verbose toolbar and I can have my docked promptbar without hunting around and it would all make more sense to people retarded by previous exposure. SW sort of has this but the UI arrangement is pitched at the type of discipline rather than the origin of the user.

          2. Neil

            First official Matt blog request on behalf of Neil….keep this number 6722374,

            Neil if you wanted send me your email

            Forget to mention, the verbose command are kind of there, but power users won’t spend that 1sec to read it.. :-)

          3. Wow! I got a number and everything. :) Thanks on behalf of all the retarded users out here :D

  3. My favorite workflow for patterns is to create the sketch first. I put the pattern in the sketch and then I draw the cutout pinned to the corner of the sketch where the little “x” that marks the reference point is. You can do anything to manipulate the pattern that you can normally do, suppress occurrences, stagger, etc. Then make the cutout feature and the pattern  using “select from sketch” at the stage where you would select the sketch plane. This way if you change the dimension of the pattern the cutout moves with it automatically. You just edit it in the sketch.

    For a hole pattern I would start the same way with the pattern in the sketch. I might put a circle in the sketch to represent the hole but it isn’t necessary, After closing the sketch I make the hole feature. At “select plane” I use “Feature’s Plane” and select the sketch as the feature. Then I make the pattern using “Select from Sketch” as above. this way I can put the sketch on to an entirely new plane and everything will follow. I can also copy the whole mess and put it somewhere else.

    1. Larry, thanks, that’s useful. I’ve had no luck trying to sketch first and then create features. I must be doing something wrong.

  4. I moved the ordered part to Synchronous (right clicking on Cutout 1152 – the final feature).

    It took about 2 minutes to move everything and a screenshot is attached. Patterns work, holes are identified as features correctly as are cutouts and mirrors.

    The problem comes when you then try to adjust anything synchronously. It is PAINFULLY SLOW.

    My point is, why would you ever do a part like this in ordered mode in the first place?

     

    1. Andrew, yeah, that was my conclusion, that it was better in Synch than Ordered. I just did it in ordered because some SW users wanted to see that comparison. There’s no reason to do it that way.

      Changes in Synch are “painfully slow”? You mean for the big pattern?

      1. Matt,
        If you try and move one of the long cutout faces it takes an age to move.

        Dan, why would this take so long when it has been converted to synchronous? Any ideas?

        Andrew.

      2. Matt, after converting to synchronous, if you try and move one of the long cutout faces it takes an age to move.

        Dan, why would this take so long when it has been converted to synchronous? Any ideas? I even exported and reimported as x_t but it made no difference on performance. Really strange!

        Andrew.

  5. Matt, clearly the performance here is not acceptable. I don’t know what is giving us such fits with this model, but I will find out. On the compact, but somewhat cryptic nature of the command bar, I am not sure if you know, but you can go to Options –> Helpers and towards the bottom of the dialog set “Vertical format” and it will go to a fully verbose panel like SolidWorks. You will likely want to “pin” that page of Edgebar having done so, so that you always have it available. This is clearly an easier to learn format, but takes up a pretty large chunk of the screen. Although its the only way to work in Works, it is an option in Edge. I think about 20% of our users use it.

    1. I’ve heard about this thing before, but when I set that option, I don’t get anything. I don’t even get the command bar. So I’ve probably got it turned off somewhere. I’ll poke around and try to find it. Thanks!

      1. After you set it, look at the left edge of the screen and you’ll see a tab with the active command name on it. Just click on it to pull it out. Then, you probably want to hit the pushpin at the top corner to leave it always pulled out.

        1. Oh, yes, thanks, very ‘Works-ish. Actually this looks great. I had a feeling what I was missing was already there. Thanks again. This will make it much easier, I think.

  6. Matt one thing i notice from the screen capture, and i wonder why some SE users miss this, you use Smart Pattern instead of Fast. This will have a major impact on the time the part take to recompute.

    http://www.soliddna.com/SEHelp/ST4/EN/feat14c.htm

    http://www.soliddna.com/SEHelp/ST4/EN/feat13d.htm

    Definitely i can see SW influence in the way the part was model, one thing i notice, many you use several planes orientations of the planes you use to create your features have different orientation.

    http://www.soliddna.com/SEHelp/ST4/EN/refplaneb1a.htm

    Here one example for plane creation

    http://www.soliddna.com/SEHelp/ST4/EN/coinplane1h.htm

     

    1. Luc, ok this was a big influence. I went through the part and changed the patterns to the Fast option instead of the Smart option, and the total recompute time is now about 90 seconds (from 16 minutes). Much faster.

      There is an equivalent option in SolidWorks called Geometry Pattern, but there was a lot of bad information given out by SolidWorks and resellers about this option which leads to people having an incorrect understanding of what it does. It is essentially the same option as your Fast option.

      I’m interested in what you have to say about the plane orientations. I’ll try to learn more about that.

      1. Going with a basic situation for plane

        Once you got your base plate, start an extrude and hover over one of the face of the base plate ( preferable to choose a large one)

        One edge of the part will be highlight to show you the Horizontal of the sketch. Also on the left of this edge, you should see a reference box. This reference box always try to locate bottom left corner of the screen.

        If you look at the PromptBar you will see that you can N B T F P this will help you change the orientation of the plane or flip the normal of the plane. This will help you maintain ( keep) orientation consistency between feature.

        Also it will help predict sketch orientation based on how you picture the part in your head.

        Also when you do a feature, you can select a plane base on existing feature as mention by Larry K. This way all features will be link together , if the first feature is edit and its plane orientation is changed, all related features will keep their relative position. That can be useful for parametric parts.

        If you want to test more, draw a sketch that contain a spline.Now try to create a plane normal to a curve, and use the F or N or B

        http://www.youtube.com/watch?v=Vrcf626eE6k

        To continue on what Larry mention. In SE  see patterns as  road map instructions. Those instructions can be independent of the model.  Making it more stable in case of model change.

        One situation that designers face, I need to center a pattern on a face, Where should i place the first feature that will be pattern?

        Notice on the rectangular pattern, you can delete the Horizontal/Vertical constraint on the lower side, This will give you the chance to rotate the rectangular pattern if need.

        More than one pattern can be placed inside a sketch if you want to centralize pattern definition.

        If you want to replicate SW pattern, use pattern along a curve to set pattern direction 1 and 2, it should do the tricks.

        P.S. you mention 90 sec it this on you brand new pc?

         

  7. OK so I am playing around with Spaceclaim 2012 and I thought this would be a good comparison test. I opened the SolidWorks file, selected the end faces and end chamfer, used the move tool. The preview is instantaneous and interactive. But when you commit the tool you wait….and wait…and wait…and wait. I waited for 15 mins before cancelling the command (which works pretty well – there is a stop button).

    All in all I’m a little disappointed in this. Spaceclaim uses ACIS. I use other apps that are ACIS based (SharkFX, FormZ and Ashlar Cobalt). I tried this in Shark and it moves the face fairly quickly, but general file manipulation is slow. No idea why Spaceclaim is so slow. It opens the file in a few seconds, graphics are top notch, move preview was instant…just the operation itself was dismal.

    So I’m playing around then with the Task Manager and all doing these kernal tasks I see only one core is active – much like SolidWorks. This cannot help.

    How long before Parasolid and ACIS are able to handle more than one core?

    1. Kevin, various functions in Parasolid do use multiple cores, but it is far from all. I’ve been trying to get a comprehensive list of them but I believe its things like shelling and hidden line detection. Not sure what else. I see it a lot in SE when creating drawing views and a lesser degree when rebuilding a lengthy feature tree. Beyond that, the stuff processes too fast to tell what it uses…

    2. I find it interesting that you would second guess Mike Payne using Acis in SpaceClaim. Mike put together ProE, started Solidworks with Acis, switched SolidWorks to Parasolid, was CTO of Dassault, and was the CEO for the company that owns Acis.

      Are you sure your multiple cores are turned on in msconfig. I use multi cores in SolidWorks and SpaceClaim.

      1. Not second guessing anyone. Not disputing the track record of anyone either. Just reporting my findings. Some operations in Acis and Parasolid are multi core multi thread aware but not that ma
        many.

        And yes I do have multi core on.

        Interesting that you say Solidworks started on Acis. News to me. Solid edge started on Acis for sure. I evaluated it at the time and it was poor compared to Solidworks in Parasolid. That is why Edge switched.

        I think it is also safe to say that licensing Acis is cheaper than licensing Parasolid. Or it used to be. Was probably also easier to implement as well.

        1. In recent years new rendering engines have revolutionised the way we do visualisation now. Part of the reason for this is making the render engine able to run all core flat out. We use Keyshot Modo and Maxwell for rendering. Using those apps turn on task manager and see all cores and threads running at 100%.

          Do the same for any modelling app like Solidworks and you rarely see more than 1 core utilised. Solidworks does use multi core for some operations like creating drawing views. Ditto for Acis apps.

          Until the kernels get up to date with hardware we will always be limited.

        2. Hi,

          You may read an interview with Mike Payne about his history and sw:

          http://www.deelip.com/?p=3523

          He has some words to Solid Edge:
          “Solid Edge is a better product than Inventor. But it had sold, if you are lucky, a third of the seats of SolidWorks. It just hadn’t been sold very well. Basically, they couldn’t get out of their own way.”

          I think the world is changing and SE has an own clear way… Mr. Dan Staples and his team knows this way and we will see and experience it!!! :)

        3. During the development period before it was released SolidWorks started with Acis but switched to Parasolid before the first release in the late fall of 1995.

          Another thread mentioned the very good interview that Deelip did with Mike Payne.  It’s excellent and mentions more about this and a lot more.

    3. Hey Kevin,

      I can confirm that SpaceClaim takes way too long in this test.  I can also speed it to up to be very fast via a workaround that’s generally useful on large parts: split up the model into small chunks, edit, and merge back.  I can also say that this performance issue appears to only happen when SpaceClaim is running ACIS, and that SpaceClaim running Parasolid completes the job in about the same amount of time as Solid Edge.

      Parasolid? But what? It turns out that we actually got started on Parasolid and ended up switching to ACIS.  We continue to maintain both kernels in-house, but we only ship on ACIS. The reason: by and large, ACIS is a more capable direct modeler.  This punch holder appears to be an exception.  I’m a little surprised, because we’ve been doing some things to speed up performance on large models.  Somehow something about that this part to be throwing ACIS for a loop.  (Probably, literally, a loop. Like a “while” loop. Ah haha.)

      But doesn’t this test show that Parasolid is clearly better?  No.  Not at all.  We have thousands of tests that run on different variants of SpaceClaim (ACIS and Parasolid, x32 and x64, on a few different versions of Windows, etc, etc) in constant rotation.  Parasolid is a very good kernel, but ACIS won our business for a reason.  We are aware of many cases where Parasolid appears better, but there are also many more cases where ACIS does the job better.  The engineering decision was to go with ACIS.

      -Blake
      (A SpaceClaim employee)

      1. Great feedback Blake. That’s a very interesting comment on running Parasolid and Acis. Kind of like Ironcad but not :-) if nothing else it shows the ability of a pure direct modeller to chop and change kernels.

        The thing that confused me was how different Acis apps respond differently to this model. Shark FX, which grew from Ashlar Cobalt opens the file a lot slower than Spaceclaim and it’s graphic performance is nowhere near as good as Spaceclaim but it performs the move faces operation a lot faster. FormZ just ground to a halt. Haven’t tried Ashlar yet.

        I’m still getting to grips with Spaceclaim btw :-)

      2. Blake,

        My understanding is that your comment is for Parasolids as it is licensed to Siemens competitors. Considering the idea that the best direct editing features for Parasolids are not for sale to SpaceClaim how would you go about assessing the true capabilities of the Parasolids kernal that SE gets to use as compared to what you get to use and make a valid comparison of the true capabilities of ACIS vs Parasolids regarding direct editing?

        1. Dave as I see it Blake is talking about functional kernel operations. Things like the way the kernel handles features like blending, shelling, local face operations, healing etc. in this respect ACIS is a very potent offering. I’ve used ACIS based systems for many years and there are many things it does better than Parasolid ( and vice versa).

          As I understand it ST does not affect the ability of the kernel to actually complete an operation. Rather, it is more of an interface and constraints mechanism. I think what Spaceclaim have done is go their own way and develop their own optimised interface to direct modelling.

          I’m trying it at the moment. I’m impressed. I’d suggest anyone looking for a direct modeller should take a close look at Spaceclaim before parting with cash.

          1. Kevin,

            “We continue to maintain both kernels in-house, but we only ship on ACIS. The reason: by and large, ACIS is a more capable direct modeler.” I believe Blake is indicating direct editing is the main topic here and this does relate directly to kernal content.

            How ST and Parasolids work together is not known to me so your comment on ST being an adjunct to and not an integral part of the Parasolid kernal  I cant answer. Perhaps an SE guru will.

            I do believe Blake and SpaceClaim have the same problem as Dassault. I believe that this is why SW will have the kernal change as Dassault scrambles to try and fix their listing SW ship. Neither SpaceClaim or Dassault/SW have access to the real goodies.

            Speaking of Direct editing and SW. You seem to have a fair amount of interest in direct editing lately and inquiring minds want to know if you are  getting a life raft prepared or are you going to stick around for SW V6 Le Stink!R-onerous Technique?

          2. In answer to the question about direct editing, I take the view that direct editing is nothing new – I was doing direct edits in 1984 in ROMULUS. It is really only since Spaceclaim came onto the scene that all the major CAD vendors realised that there was marketing mileage in direct editing. You can (technically) say every CAD system that is not history based is a direct modeller – Autocad included.

            When it comes to it, the geometry operations you can achieve doing direct edits are still limited to prismatic or analytical surface type parts. OK so you can get nice previews, and the process is more interactive but when it comes to it there is not much I can do now that I couldn’t do 15 years ago in Vellum Solids or FormZ. Extruding of faces of other parts is nothing new either – again both the above apps have had this since day 1, so I will admit I get a bit jaded by proclamations of new functionality :-)

            Blake describes a method of splitting the part into bits, making the moves on the split part then joining it all up again. That is something you can do easily in a  pure direct modeller, but it is also something you can do in any modeller. It is something I do in SolidWorks. I think the key here is you adapt your modelling techniques to meet your design objectives – not your modelling objectives – there is a subtle difference.

            So my interest in direct modelling is long standing. I don’t subscribe to a polarised workflow though – where I must use direct methods or I must use history or whatever. I use whatever fits my task. This is why, unlike Matt, I don’t have issues with direct face tools in history systems like SolidWorks. I have thousands of models where I use these techniques without any issues whatsoever. For example recently we just purchased Rhino and TSplines. The future of that combo may be open to conjecture but for us, right now, this is a winning combo. We can work in Rhino, or Modo, export Tsplines or OBJ and import into SolidWorks via Tsplines. I have future proofed this by buying Rhino – worst case, we can export from Rhino as STEP or IGES into SolidWorks, regardless of what happens with Autodesk.

            So, like others I keep my ear to the ground and try to assess how different things might benefit our workflow. I’ve seen nothing so far to make me want to jump ship to SolidEdge. I think Matt’s blog here demonstrates that there are still lots of areas that are less than ideal. It has taken 5 releases of ST to get to this stage (I am including ST5 which is imminent).  Now I find it ironic that many are prepared to play this waiting game while complaining about the lack of development with other apps.

            In the same timeframe, PTC have developed Creo with some very interesting Sub-D modelling in the core system, Autodesk have taken Fusion to new levels with Tsplines, and SolidWorks have continued to enhance their system. We are not even at release 1 of SW v6 – think what we might get by release 5? I’m not in any rush to jump ship – I’ll wait and see what actually happens, and in the meantime I’ll continue to invest in systems that give me genuine value for money workflow advantages, or that simply let me work in new ways.

             

          3. Direct edit is not new for sure. Now I don’t remember the time frame precisely but John Baker with UGS posted an article on the  SE BBS about the origins of it. He said they had tinkered with this as far back as in the 80′s but that the horsepower under the hood for mainstream workstations was not sufficient until recently.

            I agree with genuine value and what works well for me may not for the next guy for sure. I follow your trek with interest and wait to see where you will end up.

            You Remember Chris from VX? This method of spliting the part into bits was a favorite of his and it worked well  for the VX kernal to.

            I think the saving grace for many and the reason they have been patient with SE is that after all it is not a take it or leave it proposition. You can still work strictly in traditional if you wish or any other combination thereof.

            Looking at the struggle every company has to get direct editing going well it is not simple.  The problem SW is going to have though will be compounded tremendously by translation problems. I fail to see how this will go smoothly and the problems for them are far larger than just implementing direct edit. I will watch with interest to see what arises there and look forward to your future comments when they finally get it going.

  8. I too am evaluating SE.  In the assembly tutorial ‘Modelling a cover associativley withiin an assembly’ it states that ST is not an option when working with inter part links.

    Inter-part links exist in the ordered environment in Solid Edge Part rather than the synchronous environment. Once you are in the part environment, you will transition to the ordered environment.

    So I think  it is important to explore to Ordered side of SE because it seems there will be times when modelling top-down that ST wont be an option.

    Is this the case?

     

    1. Yes that’s definitely the case. However with each release of SE, synchronous gets added features. ST5 is just around the corner and I am evaluating the Beta release as a tester. Under the confidentiality agreement the testers cannot reveal the new features, but I can tell you that ST5 has some incredible new features accross the board, especially in synch tech.
      Also remember that this is only release 5 of synch tech and I am sure investing in this now will prove huge benefiits to your productivity.

      1. So let me understand this? SolidEdge using ST does not allow you to create top down assemblies, where you edit one part and others update in context? Surely not. That is a kind of fundamental design approach for most users. How can there be any “design intent” without inter part relationships?

        1. Kevin, in ST, I think there are no relationships between parts in the same way that there are no relationships between features within a part. If you want multiple parts in an assembly to change together, Live Rules can handle that, or you can select faces from multiple parts. It’s the whole “design intent on the fly” idea that allows you to change your design intent very easily. In-context is not a very flexible system for changing design intent. I think I’m describing this correctly, I’m sure someone will correct me if not.

          1. Coming Matt with some info BRB and will edit this post…

            Update 2012-05-27

            Looks like Roger beat me with a video from Siemens, Anyway, i’m sure you will appreciate this one, because it will show some of the stuff Synch can do at the assembly level to manipulate assembly components. First time i record live ( or almost) hope you enjoy it.

            http://www.youtube.com/watch?v=vqNjOSe-rf4

            I also add a complementary video showing the copy paste hole.(sorry no sound for this one)

            http://www.youtube.com/watch?v=-RB52B63vQo

            Inter-part relations are create following Synchronous philosophy where we apply relation to the 3D model.

            Again and i repeat often, Inter-part links are not an obligation or a goal to reach. Inter-part relations is simply a tool that you can use at the right time and the right place in the right context.

            http://www.soliddna.com/SEHelp/ST4/EN/intprt1a.htm

        2. Kevin

          Quite the opposite, a big part of syncs strength is top down design.  Up until ST3 inter-part copies were not linked but ST4 brought some new functionality which I believe is superior in many ways ( this video showing the functionality near the end http://www.youtube.com/watch?v=A6VPTOiJXkg&feature=related).

          Firstly it allows extruding directly from assembly faces (13.00 in video) – this is a great workflow.  Secondly, inter-part relationships are created after the fact (14.30 in video) – the command finds all of the relationships and you have the option to decide which ones to keep.

          Why do I think this is better?  Well, typically when you are creating parts top down you start off not knowing what the part looks like and creating links at this stage in order to create  geometry is a real bind as the many changes often break links.  With this new workflow you only create the links when the part is done so you get the design freedom at the front end and breaking links becomes less of an issue.

          Roger

          1. I haven’t done all the tutorials yet, or maybe they are a bit out of date, but that looks promising.  Thanks for clarifying.

          2. Luc
            Sorry for stealing your thunder! However, you video is more comprehensive (as usual) in showing the workflow.

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