Master modeling - tips & tricks

[torbjorn_heglum2]

I am normally using master models for all kind of welded constructions. Even frames are made like this, not as quick as the frame generator, but here plates and sheet metal can be included in the same model. Flexibility beats quick first design when there is a possibility for design changes (at least in my world).

So I have enclosed this model where you can see some of the tricks used to make this an effective tool for flexible Top down design. This is just the start of a HPU design, much more will be included before the parts and the assembly is generated. 

• Use a reference body (the red one) for reused parts.
• Place the master model as the first part in the assembly. Then the red geometry can be used to place next instances of parts, by joints or ref patterns.
• Make logical feature groups for various elements of the design, in this example; a frame, a tank and a foundation. When working on one of this elements, EOP is dragged to the relevant group.
• Give descriptive names to the most important sketches and work geometry.
• Give names to only the most important parameters, not more.
• Use geometry to define features rather than parameters (use extrude to or between, use combine etc rather that struggling with too many parameters)
• Define a complete body for the part in the master model, no additional features in the resulting part if possible. Then it is possible to truly control the design from one place.
• Use table driven ifeatures for Structural members like beams. Quite quick to place, and quick to change. 
• Direct edit is a compact and good tool to complete the ifeature. 
• Use sketch blocks for repeated details in the model. 
• Sketch driven patterns adds a lot of flexibility (and can be reused in the assembly). 

What I miss (at least in Inventor 2017):

• Folders in the part browser. I have made a VBA routine that can folder features for me, the functionality already is in the program.
• Possibility to create new body when placing ifeatures. Now I place a box feature as a new body before the ifeature is placed, then add the ifeature, then delete the box feature.
• Replace face (with automatic face chain) included in direct edit.
• Possibility to pattern direct edit feature.
• Possibility to extrude between sketch points (now it is possible only to a sketch point)

I hope this can be useful for others using master modeling, and I hop you also will share useful tips.

Torbjørn

(Still on Inventor 2017.4)

[jtylerbc]

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@torbjorn_heglum2 wrote:

I am normally using master models for all kind of welded constructions. Even frames are made like this, not as quick as the frame generator, but here plates and sheet metal can be included in the same model.

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Frame Generator and multisolid techniques don't have to be mutually exclusive.  The same layout part you create for defining your frame skeleton can also be a multisolid part that contains plate or sheet metal geometry.  I design frames, skids, and other such plate & tube structures using this type of hybrid technique all the time.  In this case you actually can have it both ways!

Your technique to use table-driven iFeatures instead of FG does have some advantages over FG though.  The most obvious is situations where you need a feature to be based on the face of a frame member (such as a lifting lug on the flange of a beam).  In my case, we have the BOM so automated using Content Center steel members that I would prefer the extra planes and parameters in the layout model over the BOM work that would result from making the frame members in the multisolid.  But your method definitely has some merit, especially if you've found a good way of dealing with the BOM other than manually entering it. 

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@torbjorn_heglum2 wrote:

• Give names to only the most important parameters, not more.

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A couple of other options for this:

1. Set those important parameters as Key, and use the Key filter in the Parameters Dialog to filter out the noise.
2. Make those important parameters as User Parameters, then set sketch parameters equal to them.  That way they're all grouped together in the User Parameters instead of spread all through the Model Parameters.

Also, don't forget about good old-fashioned Parameter Linking.  I sometimes use it in more complex designs to create what I call "Multi-multisolid" modeling.  Meaning that I have multiple multisolid or Frame Generator -driven subassemblies, which are tied together by linking parameters between the master parts.  One of them (typically the biggest one) usually serves as the "Master-master part", in which the most general overall parameters get stored.

[torbjorn_heglum2]

Thank you for your comments.

Interesting to hear about your hybrid models. If you have any examples you want to share I would be very interested.

FG has improved over the years, and now it has developed to a good tool. But we still find master modeling more flexible. Mixing frame members & plates and set up the required dependency between them is important for us. In the master model we have access to all features and functionality in part modelling which is so much more than in the assembly modelling environment. And we don't have to create any other parts than the master model when we are working with the design, the assembly is now postponed until the design is set and the documentation phase  starts.

Dealing with the BOM:  we use the 'Description' iProperty to define type & size of each part. It needs to be associative with the geometry of the part, so it updates when the design is changed. Manually entered values is not an option.

To handle this we use a custom iProperty as a template for the value to be put in the Description iProperty. This template string may look like 'PL [X]x[Y]x[Y]' where XYZ are parameters of the model. When the part is saved, we have an Add-in that fires and updates the Description according to the template with current parameter values.

This means that each part generated from the master model must be opened and the template must be set up. In the Screencast below you can see some examples. It is very quick to set up for parts that are parallel to the main axis and sheet metal. For parts not parallel to main axis we fake a 'flat pattern' of the part.  If the thickness parameter do not match actual thickness for the part, it will not unfold. But it will reorient to a local coordinate system where we can extract length & width.

When it comes to parameter names, I don't think it is wrong to use named parameters. But when possible I prefer to create sketches with dimensions to control the design rather than named parameters, as I find it more descriptive & intuitive.

Torbjørn

Edit: The screen cast was not displayed in the post (?) This link should work: 

https://knowledge.autodesk.com/community/screencast/0f39e750-7b98-4b0d-b61e-6def65937cc7

[torbjorn_heglum2]

John,

It had been interesting to see an example of your hybrid technique, I have thought about this but never tested myself since plates and FG type of profiles often are associative to each other in my designs.

One aspect of working with the master model is that I can leave the making of the assembly to the detailing of the design. The master model is quickly made, and due to the reference geometry it is geometrically complete. So when the master models are done, we can do design reviews, do design changes as required and complete the solution while still working on a few files.

When it comes to the BOM information for plates and beams, it needs to update when to the part geometry changes, so manually entering is not an option. In our case we use the description iproperty for cut info, and we define a template for the info going into this parameter. When the part is saved the description is updated based on the parameters defined in this template.

Parameters used is typically from a sketch with driven parameters in the part or length/width extracted from part or sheet metal. For beams not parallel to the coordinate system we make a fake 'flat pattern'. The thickness or other properties of the beam makes it impossible to unfold, but it will be oriented in a local coordinate system where we can extract length/width.

But of course, some extra work is required for each part. Open, create the template, save&close  will add about one minute more per part.

Screencast will be displayed here after you click Post.

0f39e750-7b98-4b0d-b61e-6def65937cc7

(Not sure if this screencast will be added -have been waiting for Autodesk to process this for 24 hours now. But it shows how the template typically is built)

The use of master-master parts sounds familiar. But I rarely links only parameters, I rather derive in sketches or solids used directly in the modelling. I find it more intuitive to work with geometry, rather than parameters. But of course, some user defined parameters keeping the main dimensions/parameters of the design is really useful.

Torbjørn

(Still on Inventor 2017)

[torbjorn_heglum2]

The screencast was released for publishing 

This is how I set up the associative description of a part:

Torbjørn

[jtylerbc]

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@torbjorn_heglum2 wrote:

John,

It had been interesting to see an example of your hybrid technique, I have thought about this but never tested myself since plates and FG type of profiles often are associative to each other in my designs.

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I'll see if I can find one that would be reasonable to post.  I may have one laying around somewhere that was created as a training demo in the first place, and thus doesn't represent any real piece of equipment.

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@torbjorn_heglum2 wrote:

One aspect of working with the master model is that I can leave the making of the assembly to the detailing of the design. The master model is quickly made, and due to the reference geometry it is geometrically complete. So when the master models are done, we can do design reviews, do design changes as required and complete the solution while still working on a few files.

We do essentially the same with the multisolid plate / sheet metal components, and only have the Frame Generator members as separate parts until later in a project when the drawing work starts.  We essentially ignore the FG part files (not renaming them to our company standard, etc.) until the detailing stage.  So as much as possible, we try to act as though we are doing what you actually are doing.

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@torbjorn_heglum2 wrote:

When it comes to the BOM information for plates and beams, it needs to update when to the part geometry changes, so manually entering is not an option. In our case we use the description iproperty for cut info, and we define a template for the info going into this parameter. When the part is saved the description is updated based on the parameters defined in this template.

Parameters used is typically from a sketch with driven parameters in the part or length/width extracted from part or sheet metal. For beams not parallel to the coordinate system we make a fake 'flat pattern'. The thickness or other properties of the beam makes it impossible to unfold, but it will be oriented in a local coordinate system where we can extract length/width.

For plates and sheet metal, we build iLogic rules into our templates that take care of most of this.  We have a rule in our "plate" template that simply measures the part in the X, Y, and Z directions.  The resulting values are sorted - smallest becomes THK, largest becomes LENGTH, and the middle becomes WIDTH.  In most cases, no additional work is required beyond picking the correct template file in the "Make Components" dialog box.  We have a similar rule in our Sheet Metal template that works basically the same way, but measures the flat pattern to get LENGTH and WIDTH (and simply uses the Thickness parameter as-is).

This has two advantages:

• Requires no extra setup work after exporting the individual parts.
• Does not break when geometry changes, because it isn't tied to any specific model geometry.  It simply measures the final dimensions of the part, and doesn't care how the part was built.

However, it does have one problem area that your setup may handle a little more efficiently. The system we use breaks down if the plate is oriented at an angle, rather than being parallel to the origin planes.  You will get strange results because the part is being measured in the X, Y, and Z directions while not being aligned to the corresponding planes.  For us this is relatively infrequent, so we're okay with a little extra work to fix it when it comes up.  Our process usually involves using Direct Edit tools to realign the part's geometry to the origin.  That part must then be manually constrained in the assembly instead of being grounded, since the orientation no longer matches the layout part.

Structural steel members from Content Center (whether created by FG or manually placed) take care of their own Descriptions.  We have custom families created for all of the common materials we use.

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@torbjorn_heglum2 wrote:

The use of master-master parts sounds familiar. But I rarely links only parameters, I rather derive in sketches or solids used directly in the modelling. I find it more intuitive to work with geometry, rather than parameters. But of course, some user defined parameters keeping the main dimensions/parameters of the design is really useful.

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In many cases, what I am linking is essentially a series of mating dimensions - positions of holes, lug geometry, overall widths that are supposed to match, etc.  Deriving geometry could work in many of these cases, but would often be more information than I really need, so I simplify things by just linking the parameters I need instead of bringing in entire sketches or solids when all I really need is a couple of dimensional values.  Both have their uses though, and I have been known to use both methods (in some cases, maybe even within the same model).

[torbjorn_heglum2]

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@jtylerbc wrote:

In many cases, what I am linking is essentially a series of mating dimensions - positions of holes, lug geometry, overall widths that are supposed to match, etc.  Deriving geometry could work in many of these cases, but would often be more information than I really need, so I simplify things by just linking the parameters I need instead of bringing in entire sketches or solids when all I really need is a couple of dimensional values.  Both have their uses though, and I have been known to use both methods (in some cases, maybe even within the same model).

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This is the kind of linking that we are trying to avoid, keeping it all in one master model. The info is already available in the model, and mating dimensions is often controlled by the same feature for both mating parts. I think this preserves design intent better than using named parameters, but this may of course just be a matter of preference.

Anyway, it is interesting to see that we have found different approaches to solve what appears to be the same challenge,  Top-down modeling for more than plain FG models. From the description of your method, it seems that your way may be quicker, but require more preparations up front.  Using only a master model (also for FG members) I think might be a more flexible method, i.e can be used for lager variation of designs, but probably more time consuming.

A big challenge of using master modeling as we do, was to figure out  how to do things efficient. I have found little information from Autodesk and other places on how master modelling can be used in real life.  Some of the challenges have been to figure out how to set up  dynamic BOM info in an efficient way, make the master model control the assembly - also for reused parts, and keeping the master model browser tidy enough to keep design intent clear. Now we control almost everything from the master model, only BOM info from the parts and machining after welding from the assembly.

Torbjørn

[jtylerbc]

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@torbjorn_heglum2 wrote:
From the description of your method, it seems that your way may be quicker, but require more preparations up front. 

I believe this is true.  This is one of the good things that comes from having been at the same job for almost 10 years - it's given me the ability to develop and optimize these processes over a long period of time.  There were a lot of iterations that led us to this point.  It was definitely not an overnight solution.

Part of what led us to this point is that most of our BOM automations had actually been developed before we started seriously using multisolid modeling methods.  I was aware of them and had used them on some specific projects, but I actually avoided widespread implementation of multisolid techniques for a while.  At the time, we were mostly using custom templates to speed up BOM work, while building all the parts independently.

I had developed so much to help us with our BOM/Parts Lists that I thought I was saving more time there than the multisolid modeling would save.  And I think I was right, but it took me a long time to understand how to make the two work together.  Had I understood earlier how easy it actually was to adapt my BOM automation to work with multisolid models, I would have realized that there was no reason to make that decision at all.

I'm not entirely sure I would have arrived at this same setup if I hadn't had that intermediate state of automating the descriptions of individual parts.  The end result is exactly what you said;  one or two people did a lot of up-front work to build the system, and a lot of time was spent on it.  But after that point, it saves a lot of time because none of that work has to be repeated, and more people are now using it than were involved in initially developing it.

[torbjorn_heglum2]

The master model can also control the assembly.  The first instance of each part is simply grounded or flushed with origin planes. Then the master model is placed in the assembly and used as a backbone for reused parts.

The steps to build the assembly is:

- Rename bodies. New names need to match our file name convention.

- Place master model in assembly, as Reference.

- Place added instances using patterns of master model as much as possible.

- Place the other by Rigid Joints to the master model.

So this is how we make all kind of weldments. It is quick, dynamic and true top-down design. Changing one dimension of the master model will update the whole assembly and BOM.

Torbjørn

Torbjørn

[Anonymous]

Nice to get to learn other approaches, but this seems quiet complex, if used together with other CAD users...

[torbjorn_heglum2]

You are right, this is more complex at first view.  But when the user is getting familiar with this, none so far has wanted to revert to any other way. Because what other options do we have with Inventor? 

• Plain bottom-up modelling. Easy to understand, but when a larger number of parts need to adjust to each other things gets more complicated. A weldment of maybe hundred parts and hundreds of constraints is not easy to manage. Change a main dimension and you might need to update 20% of the parts and figure out 50 failed constraints. In the end, this is much more time consuming than using a master model from start.
• Frame generator. Good tool but no support for associative plates & sheet metal.
• Adaptivity. Also a good tool, but must be used with care. Hard to trace adaptive references, design intent is hidden, when it fails it tends to blow up the whole model. 

If you know other possibilities, I sure would like to learn. 

Torbjørn

[Anonymous]

We use plain assemblies with constrained parts:

- for symetrical profiles, use the same part, they will both change length

- no problem for custom plates, sheet metal, others

- constrain profiles to other profiles, so they move along when sizes change.

Maybe our frames aren't complex enough to see your way might be faster/better.

[torbjorn_heglum2]

It definitely depends on complexity. Below is an example of a design where the update of two main dimensions changes most of the parts in the assembly. Definitively more work to change if it was modeled Bottom-up.

Torbjørn

[Anonymous]

I see, ours never get more complicated than...

[jtylerbc]

@Anonymous, the plate and sheet metal parts in your example image are pretty simple, and also fairly repetitive.  They don't seem to have a lot of geometric relationships to each other - you just have a few independent plates that repeat.

In a case like this, multisolid modeling for the plate components is possible, but may not have a lot of advantages.  I would tend to build something like this using individual parts for the plates and sheet metal.  However, I would still use Frame Generator to build the large primary frame.  Even without combining it with multisolid techniques, the FG tools would be a more efficient way of locating, sizing, trimming, and mitering the tube steel. 

If you do a lot of frame work similar to what you show here, and you've never used the Frame Generator, I would suggest you look into it.  Even if you don't go to the extent that @torbjorn_heglum2 and I have been discussing, the FG tools alone would probably be a large boost in productivity over individually modeling and editing these frame members.

[jtylerbc]

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@torbjorn_heglum2 wrote:

The steps to build the assembly is:

- Rename bodies. New names need to match our file name convention.

- Place master model in assembly, as Reference.

- Place added instances using patterns of master model as much as possible.

- Place the other by Rigid Joints to the master model.

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This is essentially the same as what I do, with the following minor tweaks:

• Bodies are renamed, but are a truncated version of our real file naming convention.  The rest of the name is added in the "Make Components" dialog box.
• I typically create the master model using the "Make Layout" command.  This command, run in an assembly, creates a part that is automatically grounded at the origin and set to Phantom BOM structure.  Use of this command is also why I tend to refer to the master model as a "layout part".  This is fine as-is for a Frame Generator-only assembly.  If it's a multisolid, I change the layout part to Reference since the Phantom type still affects mass.
• I've been using Inventor for well over 10 years, so I used it for several years before Joints even existed.  Although I use them occasionally, I've never really incorporated Joints into my work habits.  I tend to attach the manually-located parts using three Flush constraints to the master part.  Your way may be more efficient here, and I should probably try it out.

[johan.degreef]

If you could make a video doing your thing from scratch with some comments to clarify what and how you do it. I would sure be interested to watch it 🙂

[torbjorn_heglum2]

I may try to make a video of this, when I find time. For now you can see the the master model enclosed in the first post. If you have any questions to this model you can post here, and I will try to answer.

Torbjørn

[cadman777]

@jtylerbc 

Can you use Linked parameters in a FG assembly?
I can't in Inventor 2010.

That's always been a grip for me b/c it severely LIMITS what you can do with FG.

Example of what I mean:

[jtylerbc]

It's been a very long time since I've touched Inventor 2010.  I don't think this is different, but I could be wrong about that.

I tend to build my layout part in such a way that my need for offsets is minimized.  This often makes the layout's sketches more complicated, but simplifies the resulting assembly because I don't have to adjust offsets.  Partially because of that, it had never occurred to me to even try to do what you're describing.  So I attempted to test it, and did not have any trouble doing so.  I just manually typed in " = TestParameter" into the box, and all was well.  The parameter I tested with was a linked parameter.

If you have tried it and it didn't work, what was the specific issue you ran into?