Family of Parts and Simplified Parts

Solid Edge has two separate functions that combine to do the equivalent job of SW Configurations. I’m just figuring this out, so it seems that other SW users probably haven’t seen this yet either. SW users use configurations in a lot of different ways. We use it to simplify parts, and we use it to make variations of a part. Solid Edge can do all of that, it just does it a little differently, and it uses the Simplified Parts and Family of Parts functions to do it.

Let’s start by seeing some of the details of Family of Parts.

We’ve talked about them here, but I wanted to go through the exercise of actually making a family of parts and putting a couple variations on a drawing. I also want to clear up a few things that I think people who haven’t used Solid Edge might be confused about.

Can you use Family of Parts on Synchronous parts?

Yes.

You can create dimensions on synchronous or ordered geometry, and drive the dimensions with a table.

If you want to turn features on and off (suppress/unsuppress), you will need to use Ordered features.

Can you use tables to drive FOP?

Yes, in fact, this seems to be the preferred way. It doesn’t look like you can use Excel, but tables are definitely doable. A Family of Parts table looks like this:

This is pretty nice. As far as I can tell, there is no cryptic syntax at play here like in SW Design Tables. You can even place different configurations in different places (notice the Path fields). The FOP table enables you to change dimension values, suppress or unsuppress features, control text based properties, control Live Rules, and any relationships created in the part.

One really cool thing about the FOP table is that as you mouse over values in the table, the values highlight in the graphics window. This just feels worlds beyond SW and Design Tables. Design Tables always feel so fragile and tentative. If you click on the wrong thing or in the wrong place, the whole thing could disappear, or it might screw up your table. Solid Edge just feels a lot more solid in this regard.

Here’s one I don’t quite understand. In addition to the FOP table, you can also access a Variable Table. I’m guessing that the Variable Table is for controlling a bunch of dimensions at one time, and probably intended for use when you’re not using FOP. You can access all the variables on the Variable Table from the FOP table, but the Variable Table has some extra columns, such as Rule, Formula, Range, Expose, Exposed Name, and Comment.

You can rename dimensions listed under the PMI heading in the Pathfinder (FeatureManager). It’s nice to have all the dimensions listed in one place like this. Dimensions that aren’t named get default names like V3406. This is a really nice way of handling things.

Oh. Here’s one that’s even better. You can select from the RMB menu to show Values, Names, or Formulas. Showing formulas shows both names and values. And then of course you can show or hide specific dimensions using the PMI heading in the Pathfinder, with those little checkmarks next to the listed dimension names. I think this is very nice. I’m not sure why people seem to give the impression that SolidWorks configurations are better than this.

The one thing that I think could go either way is that SolidWorks configurations are all in a single part, and FOP makes a set of completely different parts.

Simplify

Solid Edge has this tool called Simplify. You find it in the same place where you find the Synchronous and Ordered options. This is a little confusing to me.

Reading the Help on Simplify shows one of the big differences between Solid Edge and SW. You will rarely if ever find a statement in the SW help that tells you what the conceptual goal of something is. For example, under Simplifying Parts, the Solid Edge Help has this to say:

The commands in the Simplify Model environment allow you to reduce the complexity of a part so that it processes more quickly when used in an assembly. The ultimate goal of part simplification is to reduce the total number of surfaces that make up the part.

It’s nice to know that fewer faces on a model will help it to process faster. This is something it took me a while to learn in SW. I don’t get the impression that Solid Edge is trying to hide information from users the way that SW does. I think SW things they are making it simpler by giving the user less information. But they are wrong, they are just confusing people. Anyway, I’m getting a little distracted here. It’s rare enough to find something encouraging in any software Help file.

The Simplify “environment”, I suppose it’s called, is initially a little strange. They advocate using features to block out other features. So to eliminate a fussy detail, you might extrude a block over it. So additional features added under the Simplify heading in the Pathfinder are kind of like a special use configuration in SW. In the image to the right, I deleted the 7 faces of a hexagonal cut in the top of this part instead of suppressing the cutout. I’m not sure this is really the intended workflow, but it demonstrates the use of the Simplify environment.

You can also save a simplified version of a part to an external file. Which ever method you use, simplified versions of parts can be used in assemblies or drawings.

Hmmm. I’m left wishing that the Simplify environment enabled you to use Suppress. Other than that, I’m finding very little use for the Suppress function in Solid Edge.

 

33 Comments

    1. Luc,

      Cool, excellent stuff you’ve got there. It’s going to take some time for me to absorb all of this. Thanks again.

  1. Matt, you might find this helpful: http://www.youtube.com/watch?v=Am5pDlXIKFU&feature=plcp in what Simplify Part does.  I did recognize in this video that we don’t do a very good job of outlining “why” before we start.

    As you stated, Simplify is there primarily for performance reasons.  A simple example is a gear.  If you are working on a 5000 part assembly that has gears in it, it is unlikely that you need to see the gear teeth when you are not working on the gear.   In this case, you would use simplify to “turn off’” the gear teeth so they are not processed and therefore do not consume CPU or graphic card cycles.   In fact, in the Engineering Reference tool, (that creates items like gears); Solid Edge automatically creates parts as simplified.  These are tools intended to improve performance on massive assemblies.    It makes most sense on parts that are used in multiple places since it does take some time to simplify the part.

    Kim

     

    1. Kim,

      I’m impressed with Ally’s willingness to put stuff out there for the whole community to benefit from. The information is very useful, and for this particular video really shines a light on some topics I didn’t know about.

      1. Matt,

        AllyPLM is our partner, and I have to say they have been super with information between their Lunch Bytes, posting to Youtube, participating and supporting user events and direct customer help.  In fact, I believe at least one of their staff will be teaching a seminar at Solid Edge University on Solid Edge Simulation, and I hear she is super knowledgeable on using it.

    2. Hi Kim,

      I completly agree with you.

      I (we) use it everytime. If you put a “complex” part into an assy, this representation mode is very useful for better handling. The strength point of this is that you can use it for imported parts. Fortunately the Standard parts (bolts, nuts, etc…) contain this simplified mode!

      I’ve linked a short video about my workflow:

      http://www.youtube.com/watch?v=0DeXUAJcVT4

      BR,

      Imics

       

      1. Imics

        Great video.  I never knew you could delete features in the flat pattern.  Great to see real parts in a real workflow.

        Roger

        1. In Sheet Metal, the Flat Pattern is its own environment as well.  In the flat pattern, I add holding tabs and other manufacturing geometry that do not appear on the finished part.

  2. The Simplified mode can also be useful for creating an “as cast” version of a part where the Design mode can be used as the “as machined” version.

    1. You can, but I would argue that it is not the best practice.  Using an “INSERT PART COPY” is probably the better method to model as-cast and as-machined versions.

  3. Matt,

    We also have a Lunch Byte on Variable Table.  For some reason it was not on our Channel, but Ben just uploaded it.  Maybe it will shed some light on this tool.

    One of the more common uses is as kind of an Excel Lite.  You can always connect to Excel if you need all the functions it provides, but the Variable Table gives you many similar functions inside Edge — setting up relationships and variables, etc.  Many things you may need Excel to do in other systems, can be done in the Variable Table.

    http://www.youtube.com/watch?v=GlgfuV6mLls&feature=plcp

    Kim

  4. Matt, this is a good read and its nice to see a new user perspective on things. I think there are couple important points to note here, one conceptual/technical and one about how Solid Edge develops software.

    1. Simplify is found with Synchronous and Ordered for a reason. They are more parallel than you may realize. Each of these has its own set of allowed commands (what we call an environment) and they go one after the other in the feature tree. Synchronous computes first, then, Ordered. This results in the “Design” body. Then simplified computes and results in the simplified body. The key advantage of having simplified be a series of operations on the design body is that suppressing features has consequences — you cannot freely suppress what you might need to without “breaking” other features further down the tree. So you can’t always suppress yourself into a simplified model. Think about a heat exchanger. You don’t want to “suppress” the fins. You want “represent them in a different way”. So you can draw a big ole extrusion over them (eating them up) and that is a really good representation in a very large assembly.

    2. We’ve often thought of other systems a “toolboxes” and to the extend possible, we don’t want to be “a bunch of tools the user has to figure out how to use to do something useful”. I think configurations are a great example of this. Will configurations do both Simplify and Family of Parts? Yes, for many cases. However, rather than building one hammer that can be both a screwdriver and a hammer, our approach tends to be to look at the problem and craft a solution. The needs of part simplification to reduce assembly complexity are DIFFERENT from the needs of a family of parts. Key to simplification (in our opinion) is the ability to use your existing model, but draw what you need to represent the simplest useful representation. Another difference is that clearly a simplified model must be part of the same file as the design model (they are not different part numbers, they are just different representations of the same thing). Whereas family of parts (in our opinion) should be different files — they need different part numbers, you may need to revise each independently, you may have access rights to one or the other, but not the master and so on.

    Anyhow, kinda longwinded, but I think important. Solid Edge spends A LOT of time designing functionality to solve a particular problem and we try to avoid generic tools that solve 90% of several problems but 100% of many fewer.

    1. And where I get the other SE users upset with me, you can open the child FOP member file and treat it like an “original” file.  In other words, open the file and it has a single feature.  Let’s call it starter geometry.  I can add and remove material to that as my hearts content without affecting the Master or the other children.  I can create simplified versions of it.  I can render it a different color or apply a different material.  There are some seriously powerful things you can do with FOP as separate files that are harder to manage when lumped together in a single file.

      1. And you can even insert FOP members into another FOP Master to generate even more children…

        1. Well, that’s just really messy and now you’re talking about some serious file management issues.  I know you were being a bit sarcastic with that answer.  Although it is technically possible, I don’t know anyone who would actually do that.

          The reason I brought up my workflow that annoys people is because it is very powerful.  Like a lot of conversation in these discussions, users think they need to define EVERYTHING in the master part and then either edit a variable or suppress a feature to make the children.  With SE FOP, that is not the case.  You can include as much, or as little, geometry in the master as you want and then finish the part (features) in the child.  Using this workflow, I don’t have to suppress any features from the master to make the children, I never model them in the first place.  They get added later.  When dealing with ordered, history-based features, this may not be an acceptable workflow because of parent/child dependencies.  But in that case, the parent child dependencies may prevent you from suppressing the feature also.  No problem with FOP.  Open the child and toss and extrusion or cut over the feature you wanted to suppress but couldn’t.  Congratulations, the geometry is now “suppressed.”

  5. So you cannot suppress features except in ordered mode? Interesting.

    One of the important used for configurations in SW is creating machining stage models on complex CNC jobs. For example a part might require 6 or 7 stages in the cut cycle. What a lot of SW users do is model the part ad it would be machined. Then turn off features to correspond to the CNC stage and save as a configuration. These can be taken through to a drawing. One part. Like it or not configurations are a critical part of many many SW users workflow.

    1. Hi Kevin,

      SE synch is not a history based modeling technic, so you cannot suppress features, but you can detach and attach and this is important if you use imported models.

      But you can “suppress” and “unsuppress” any part of the 3D imported or synch model if you use mixed mode! This is my favorite “top gun”.

      Here is an example (imported model with suppressed slot and without it in FOP):

      http://www.youtube.com/watch?v=ZOnf_UZ88yg

      What works on imported model it works on “own” model!!! ;-)

      BR,

      Imics

  6. It has been a while since I’ve had parts so complex that I created a simplified representation of them.  I mainly do it on springs and other parts with a lot of radii or helical geometry (extrude a simple cylinder, or hollow cylinder, over the helix).

    In practice, you rarely want to save out the simplified part if you plan on using it in an assembly.  When you open an assembly, you have the options to show simplified parts or as-designed parts.  Obviously, using the simplified version improves performance by not having to render as many faces.  But, when you add assembly constraints, the geometry is constrained AS-DESIGNED regardless if you are showing the simplified assembly.  Likewise, the physical properties (mass, moments of inertia, CG) are all calculated from the as-designed geometry, not the simplified version.

    If you Save Out the simplified version to a file, that is considered the as-designed version so you lose the background data.  The positive, you can send that Saved Out part file to a vendor as a “shrink wrap” version and hide all of the background data.

    1. Scott,

      Yeah, I’m starting to see that FOP has a somewhat different application than SW configurations. There is a lot to keep track of here.

      I’ve been wondering how Solid Edge users do “master model” technique, although I tend to use this mainly on surfaced models rather than mechanical models. Any input there?

      1. Matt,

        I typically model my parts that are to be cast, as a fully finished [machined] component…essentially becoming my “master model”, then I make a new file, insert a part copy (at which point I can add the shrinkage allowance) and add/remove any/all features that are relevant to the casting process model only.

        1. You see to me this sounds like a backwards step. Configurations allows you to do all this in one file. In the drawing you just change the configuration used. Done. Like I said. This is a core workflow for many SW users. I’m surprised ST has nothing similar.

          1. Hi,

            I think, the SW Configuration has advantages an disadvantages! The all cnc workflows are in only one file. That is cool. But… What is the size of the files?? We and SW users know there is a serious problem with SW file size… SE offers individual files to avoid this problem.

            From Dan:

            “Whereas family of parts (in our opinion) should be different files — they need different part numbers, you may need to revise each independently, you may have access rights to one or the other, but not the master and so on.”

            I absolutelly agree with he!

            BR,

            Imics

          2. Kevin, yeah, I see what you mean, but if you think of what you actually do with configurations, Solid Edge methods cover all of that. In SW configs you make simple versions of stuff, and different part numbers.

            And then look at the default implementation of Toolbox that uses configurations. It’s a total disaster because you wind up with file management issues – same file name with different contents between Toolbox users. You would never have this problem with Solid Edge’s method.

  7. I’m sure there are pros and cons to both methods. Managed properly configurations is very flexible. Sure if you balls up part numbers and configs you are screwed – but the same applies to any system. If you take an example of what I’ve been doing today – generating fitting instructions for a product we designed for a customer, we have one master assembly file and 5 sub assemblies, with 12 configurations – stage 1/stage 2/stage3 etc. In each one we show/suppress/move different parts, or change configurations in the sub assemblies.

    So for this assembly with just 27 unique parts, 1 master assembly and 5 sub assembly files, I reckon you would need over 200 part files/assembly files in various stages to do the same task. In that context the scope for complexity and error is high.

    1. Assembly Families are not separate files, they are handled inside one file, so you wouldn’t need that many files…

    2. There is absolutely no doubt that both approaches have their merits but what I find most interesting is that the differences aren’t because of technical limitations but are driven by each companies philosophy to software design.

      “So for this assembly with just 27 unique parts, 1 master assembly and 5 sub assembly files, I reckon you would need over 200 part files/assembly files……”

      Kevin, forgive me if I am making assumptions but I’m not sure you understand that SE deals with part and assembly configs in a totally different way to SW.  SE uses Assembly Configurations (basically hide/show part), Alternate Assemblies (parts positioned in different configs) and Families Of Parts (multiple variations in actual part geometry).  From your description it sounds like you are using the first two, in which case SE would still only have 1 master and 5 sub-assemblies.

  8. You are correct Roger. I don’t have any understanding of how SolidEdge handles assemblies. I’m just going on what I’m reading here. I think the confusion is the family of parts thing. Maybe there is a video online somewhere that shows this?

    1. Kevin here some info

      http://www.soliddna.com/SEHelp/ST4/EN/famprt1a.htm

      http://www.soliddna.com/SEHelp/ST4/EN/famasm1a.htm

      You mention in a comment  “…I’m surprised ST has nothing similar. …” my self I was surprise that SW part configuration reside in one single file and wonder why SW did not have FOP like Solid Edge ;-)

      Find this from Ally PLM

      http://www.youtube.com/watch?v=ig7dHyQp3X8

       

      Matt to answer one question about master part design…

      Master model design  is done using Inter-part copy. You create the model mock-up then you derivative other parts from the master

      http://www.soliddna.com/SEHelp/ST4/EN/intprt1c.htm

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

       

  9. Another great use of the Simplified model is to use it in Simulation. Sometimes, we can save an huge amount of calculation time by just removing some details of the model that are not important for the simulation study. Reducing the number of faces to be meshed it’s an huge time saver and the simplified model is a great way of doing it. Just another use for the Simplified model.

    CM

  10. Matt

    Simplified parts are not really anything like family of parts. To really understand the value of simplified parts you need to explore how they work in assemblies. That is where their real value is. Imagine being able to turn on and off all the little features of every piece of hardware in a machine or all them details of imported components at will.

    Try to get your hands on a very large assembly and manipulate the view with the simplified parts on and off. I have seen huge differences in the time it takes to spin a model and zoom in on something. There are also lots of nice settings to control when a part is simplified or not. For example you can set a default to always use them when opening a file or never use them when placing a part in an assembly. You can even work with a display configuration in assembly using simplified parts then display it on the drawing with the designed parts.

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