Best workflow for structural member design?

[cadull_rb]

Following: http://forums.autodesk.com/t5/Autodesk-Inventor/Incomplete-part-update-when-sketch-pattern-count-cha...

Thanks Paul,

We use structural members connected with brackets and fasteners. Our ordering system handles length, colour and hole punching separately for each line item. Colour doesn't affect structural design and hole punching we handle with an add-in. The length of a structural member depends on the overall size of the design, it's location within the frame and the requirements of the connecting brackets.

We would like to maximise the reuse of design, both parts and assemblies. Since each project is a custom design and only used once, we would like to leave any adaptiveness in place so that the assembly can be copied and adjusted to suit another project.

In summary, features we would especially like to combine are:

 - lengths of structural members change based on higher design elements

 - ability to select the size/thickness of structural members

 - level of detail to optimise viewing and simplify drawings

 - reuse of parts and (sub)assemblies

Adaptive assemblies: succeed initially, especially when first being constrained, but fail later when the assembly becomes more complex or when the parts need to readapt to a change in size. Doesn't like level of detail changes.

Flexible assemblies: slow, regularly need to drag items to force an update, be wary of constraining to assembly origin.

Multi-solid parts: minimal usage due to reuse of existing parts.

Skeletal modelling (sketches): cannot use a common origin due to part reuse. Placing key geometry in sketch blocks allows positioning when derived, but this is painful to work with and the assembled parts need constraining back to the sketch elements. Patterning of sketch elements isn't reliable.

Skeletal modelling (solids/surfaces): still testing, but seems promising as the workflow also incorporates a simpler level of detail that we need for many of our drawings.

Custom iParts: members are derived so cannot change base geometry. Currently using a template part that is an extrusion of a custom iPart sketch exported by attaching an iMate.

iCopy: could really make use of a feature like this. Would like greater control over the output file names. Doesn't seem to like parts derived from multiple parts (displays a red question mark beside the derivation, although it still seems to work and eventually disappears). Doesn't seem to like custom iParts, although table activation still works (always displays the red question mark next to the iPart derivation). Question the reliability as it uses adaptivity. Yet to test in conjunction with solid skeletal modelling.

[Jon.Dean · Accepted solution]

I think the reason why this thread has been quiet, is because you are addressing too many issues.

I was wondering if you had installed Inventor 2013 and if so, have any issues been addressed?

Jon

[cadman777]

cadu,

Did you ever get an answer to your inquiry?

I'm interested in what you discovered, since I'm having the same problems w/Inventor.

It seems to be unable to work between the applets to accomplish STRUCTURAL DESIGN AND DRAFTING.

[cadull_rb]

Hi Chris,

At every turn, Inventor features seem promising, but have limitations or issues that make them unusable for this purpose. If your designs are small enough (less than 50 frame members) or you have a limited range of fixed-size designs then using built-in features like frame generator and/or iLogic to control the members is a possibility.

We ended up developing an addin to support the following approach.

1. Create a library of reusable design components.

a) Create content center parts that are suitable for use with Inventors frame generator.

b) Create connection assemblies that represent the possible interactions with frame members. The frame members are represented in these connections with a short reference part. The connections contain cleats, bolts and other components to attach to the members. They can also include notch parts whose geometry will be cut out from the generated frame members.

c) Create manufacturing drawings for cleats and custom sheet metal folding.

2. Use the library components in each design.

a) Create a reference envelope (solid parts) to constrain the overall design.

b) Place connections in assemblies and constrain key connections to the reference envelope. Our addin supports an enhanced version of iMates that assists with the creation of these constraints.

c) Place constraints between the frame reference members to align each connection. Our enhanced version of iMates has special treatment for frame members to make it easy to join the compatible connections.

d) Generate the frame members between the frame reference members in the connections. Our addin does this automatically and includes customisable notching and hole punching for bolt locations.

3. Create engineering, construction and manufacturing drawings.

a) Inventor drawings are too detailed for engineering drawings. We currently do these in another program, but have an idea to generate thin rod members between the connections that will show as lines on the drawing with simplified BOM, labels and part table.

b) Construction drawings are from the generated frame members with some included sketches from the reference envelope parts. Our addin supports an automated design view representation setup to speed up the selection of members to include in each drawing. It also sets BOM labels to match the product that will be purchased.

c) Our manufacturing drawings are created at the library level. We don't require drawings for each member.

4. BOM, pricing and purchase orders

a) Our addin transfers the BOM to our automated job management system that will generate cost and sale prices and send purchase orders to our suppliers. A BOM comparison is provided during the transfer to detect issues and evaluate any changes. The purchase orders include information regarding the generated members such as label, length and hole punching locations (notching is performed on-site during assembly).

This approach is fairly reliable and is possible using standard Inventor features, but can take considerable user time to follow manually. To support the variety of frame members and design configurations in our library we use iAssemblies. These are the one source of annoyance and the greatest time waster in our process due to Inventors insistence on modifying perfectly good and up-to-date files. Combine this with Vault in a multiuser environment and we have no end of headaches. (Any Autodesk employees reading this - please fix!) We have several features in our addin to help users recover the mess which, along with the changes in Vault 2014 SR1 and Vault 2015, allow us to slowly work around this problem.

Regards,

cadull

[cadman777]

cadull,

Thanx for your detailed analysis.

I've come to the conclusion that there are only 2 pathways to take using IV for structural:

1. Library which is manually assembled to a skeletal sketch, or

2. Your method: Library which an SDK app assembles, and use "checkers" at the end of the process for validation and correction.

#2 costs too much for a small operation, and #1 is a lotta work per job.

The dilemma always is: Do we waste money and time trying to use IV with an industrial steel programs such as TEKLA, SDS2, etc?

Also, I found a huge problem w/generating fabrication drawings, unless they are already created in a library. However, those too need touch-up. But it's quite a time-saver to have a drg library.

The fact that you tied the whole system into your accounting/ordering/purchasing departments is quite an accomplishment!

Your success story has given me something to think about. My neighbors are programmers, and their son in college wants to work w/me on an app for this. Maybe I'll take him up on it and see if we can make something of this? There's nothing better than using one program for all parts of the process.

Thanx for sharing your experience.

[cadull_rb]

Hi Chris,

After 3 years of part library and software development, we have some way to go before seeing a return on the investment. As part of a highly automated business process, the Inventor solution has a lot of potential to integrate further into our business model. It replaces a completely manual process (2D drawing and counting screws) and a reasonable part of our implementation timeframe was making our library to cover existing designs.

If you decide to create an addin, first you need a process to follow that works in Inventor. Second, you need to be aware that some parts of Inventor do not have an API to automate them (significantly, frame generator). Lastly, the Inventor API is easier to work with if you only run code in response to a button press. Code that runs automatically, say during a model update, is more difficult to manage.

All the best with your endeavours.

Regards.

cadull

[cadman777]

cadull,

Thanx for the info.

I'll take it under advisement.

Yes, I want to automate the manual tasks in a way that catches errors and doesn't create them.

Can I hear you saying, "good luck w/that"?

I remember when I was on DOS 3.5, how I kept 'banging the drum' of file interchangability. It was a matter of common sense, not "wish list". Everybody and their brother kept saying, "yes, yes, wait till next release of the software". So we spent the money and .... well, here we are almost 30 years later (yes, THIRTY YEARS), and I'm still waiting. After a few years and 'trends', I began to realize it was all marketing lies to keep us on the hook paying for everybody's software R&D, so I quit hoping for the impossible a LONG time ago!

Cheers