Help Me Identify Master Model Techniques
Before embarking on this design project, I want to make sure I understand the Master Model techniques available in Solid Edge. Regardless of the specifics of the project, this is the type of decision you have to make early on in the process. It affects the workflow throughout the rest of the project, so getting it wrong off the bat would mean a lot of “learning opportunities” later on if you know what I mean. It’s true that you learn more through failure than through success (by which measure I should be pretty smart by now), but it might not be the best idea to actually plan to fail. If I learn something up front, then I still learn it, and avoid the public embarrassment.
So. Master model. People define this differently. Some use the term “skeleton”. I have two different techniques that I call Master Model techniques.
The first is where I use a sketch in the assembly, and model parts around the sketch, such that the sketch drives all of the individual parts. This could also be called skeleton or master sketch. In practice I don’t really do it that way. The way I really do it would be to start a sketch in a part, and then put the part into several individual parts. If you could just have a stand alone sketch by using something like an external block that could be shared between parts, that would be great. One problem I see with this is that it is going to turn into an Ordered workflow. I don’t see a way to use a sketch to drive Synch parts. I think we established earlier that this can be done through Family of Parts, which would seem to work well. Ideas here are most welcome.
The second is to model the major shapes in a single multi-body part, and then split it all out to individual part files. This is the technique I use most, and I think it is compatible with a Synchronous way of working. Except the split feature might have to be an ordered feature. Splits can happen by sketch or surface body. This method starts out intensely multi-body, and transitions to individual parts, then to assembly modeling. The problem with this is that we might end up needing ST5 with all of its multi-body glory to complete what we start. I know ST4 has some multi-body capability, but I don’t want to get into massive work-around mode if we don’t have to.
Why use Master Model and not something like Inter Part (in-context)? I think with Inter Part you’re still stuck with an ordered only workflow. Some parts could be synchronous, but they would be ones you don’t want to drive from the master model or master sketch. Another reason is the file management. With Inter Part, if its like in-context, you always have to make reference to the assembly. One part only relates to another through the assembly. If you’re inserting one part into another directly, you don’t have to worry about the assembly, it’s just part-to-part. This simplifies things, and – when you’re working with an ordered workflow – speeds things up (or really just doesn’t slow it down as much, depending on how you look at it).
I guess my question to experts out there, is what technique would you recommend? Family of Parts? ST4 multi-body? Wait for ST5 multi-body magic? The body shape is clearly going to need to be ordered surface model, but the mechanicals could be synchronous. I’d like to drive the layout with a sketch to be able to place wheels, plan the overall design in 2D basically, and reuse that 2d to drive the assembly and parts.
R&D context here- “Virtual Components” sounds like something absolutely fantastic when you get to that point where you realise that you’ve come to effectively the final design but you want to redo it all because it’s a complete mess. Actually as I type this I realise it would only be handy if you were using history only based modelling… ah well.
Dan,
I agree that a assembly sketch won’t help you always (linking to it with a lot of parts will make your ass’y very slow, so don’t use it). However for the body-parts of this you are almost required to use a master as you want all curves and lines to be continous over the different parts (bodypanels, etc).
First of all, I think it helps to take a step back and understand where “master model” or “design intent” is going to help you versus hurt you. I’d be a little careful with the assumption that (some people make) that having a single assembly sketch driving everything is going to help you. The issue is that it “captures design intent” but too early, too much (IMO). As we’ve discussed before, your intent changes as you go and to think that its all there right up front at the time you create the sketch and the parts is a bit presumptuous (of the CAD system). Rather, blind alleys and design snafus will invariably get in the way (or are a glorious part of the process, depending on how you look at it).
So you want the assembly sketch to be a useful part of the design process, but you want to “capture” relationships between the parts at the time that makes the most sense. That is the point of the command we introduced in ST3 where in Assembly you can tell one part its a child and another is a parent and we’ll go find AT THAT TIME, the relationships that make sense. I think its called “Create Interpart Relationships” or something (don’t have SE handy right now). I would definitely check this out.
Another thing to definitely use is Virtual Components. Here, you build your “shopping list” of everything you need to design. It has an outline editor like Powerpoint where you create your “BOM” of things to do using tab indent and that kind of thing. Then you do the 2D layout of your design. Then, you associate each 2D with a line item in the shopping list BOM. Then hit Publish and voila it creates all the part files and moves the sketches into them ready for 3D creation. It’s really kind of magical even like 7 or 8 years later (It was invented in Version 16), yet highly underutilized. I’d suggest you definitely give it a go for this. (PS>Works well in conjunction with Create Interpart Relationships command previously referenced).
Or, as is common, use a combination of techniques…
I would suggest that a skeleton file is best for clear planes and axes. For organic surfaces, another technique might be best, such as a master model, or master outer surface.
I am still finding my feet with sync, but another way is to modify a part in context through the assembly using sync to move faces to snap to key points in the skeleton file, but without setting up inter-part copies. Inter-part can be sync though. Insert part cannot.
Peter.
BINGO!! Neil you are absolutely right. If they are worried about revealing secrets have Matt sign the NDA and give him ST5. I have pondered the insanity of having him do this in ST4 and making him learn things only to have to relearn some stuff in less than a month. It will take him at least as long as from now until RTM for ST5 to do this so cut him loose on the stuff everyone is going to be wanting to know about anyway. In less than a month who will care about ST4 and earlier anyway except those on maintenance whose companies drag their feet on implementing versions. Certainly no prospective customer will give a flip about past versions.
ST6 is supposed to be about surfacing anyway from the scuttlebut I hear so it would be correct to start finding out shortfalls in ST5 as soon as possible as prudent planing on what in part needs to change for ST6
Perhaps they will allow you to use a prerelease build of ST5 to take full advantage of multibodies? Might be good advanced publicity/promotion as well. Of course its up to you if you want to work as a SE novice with something thats possibly a little buggy as well… Be interesting to see how you get along reproducing that swoopy body work. My impression is it will be ‘challenging’ for SE. I guess its a good opportunity to prove the ID doubters wrong. 😉
Maybe not very ST but the following method works for me:
1. Create a master model
2. For every new part just include the whole master model (as solid or construction) and include the needed geometry to create your part-model.
3. Put all parts in assembly (use shift-lmb) as grounded parts.
Splitting the part is an option but this isn’t as flexible as above method.