Frame generator: How to Notch a Frame without another FG part?

[xenocatalyst]

Hello,

I'm giving Frame Generator a really good go, assessing whether it fits into our work flow.

I really want to like Frame generator, It look really good on the surface, but the deeper I go the more limitations I find.

Here is one that I'd like some input on. Notching.

Frame generator (FG) will create a notch with another FG part, but not a non-FG part.

How do other people do it? What the best way to achieve this?

Here is an example: A cleat plate in a steel section (shs).

I have edited the FG generated part file, created a sketch on the face, and extruded a subtraction through the section.

[blandb · Accepted solution]

You can switch your selection filter to part priority, edit the tube in context of the assembly by double-clicking. Now, expand modify command and choose Copy Object. Copy in the plate as an adaptive surface. Next, use the sculpt command and use the surface to cut the tube. Finally use the Thicken/offset command to make the cut out whatever distance wider. You will need to do the offset on the top and the bottom. Maybe set that as a parameter called "Plate_Clerance" or something. This will update the cut out if the plate changes location or length. If you know it is done, then you can turn the adaptivity off, or not make it adaptive when you first bring in the surface. That is just one method.

[chenj]

Hi，there is another way:

First edit the FG generated part file, use the “Modify>Copy Object” command to copy the plate part as a surface,and then use the "Split" command to notch.

[xenocatalyst]

Hi, Both of those work well, though I prefer using sculpt as it allows for using multiple selections in the one operation.

I wonder what other methods there might be?

[pcrawley]

Make your cleat plates with Frame Generator - then Notch works perfectly.

 

While manual modelling features is OK - mixing them with FG often ends in models not behaving as expected.  e.g. A Sculpt feature which removes/adds material to the length of a FG part will not update the G_L (cut length) parameter, and you may find your cuts lists are incorrect.

 

If you don't have some "Flat" in your library of steel sections, you can add the appropriate size (width and thickness) - then when you're sketching, just add an extra line wherever you want to place the plate.  Once you've placed one cleat plate and added the necessary holes, you can reuse it (providing you have the correct length of line in your sketch).

Although I'm huge fan of Frame Generator and won't hear a bad word against it... 😉  I know that if your primary objective is to do structural steel design and detailing, Autodesk's Advance Steel is a much better bet for many reasons.

[AIR_123]

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If you don't have some "Flat" in your library of steel sections, you can add the appropriate size (width and thickness) - then when you're sketching, just add an extra line wherever you want to place the plate.  Once you've placed one cleat plate and added the necessary holes, you can reuse it (providing you have the correct length of line in your sketch).

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Interesting solution! Thx

Where do you do this customization of profiles? In custom library?

[pcrawley]

The "Custom" Library is a bit special - it contains end caps for the structural steel sections.  Although you might think end-caps would be of limited use, you can make them oversize and they become foot plates or joiner plates.  I guess the best way to describe them is that their placement requires the selection of the end-face of a structural section - and they are placed on (or offset from) that face.  The Custom library isn't like the others - you won't find steel shapes in there, and there's nothing to see in the Editor.  It's all parametric shapes which are built to suit the FG member you attach the end cap to.

Content Center Editor is where you do the editing.  (It's no more complicated than editing a spreadsheet - so 'customisation' makes it sound more complicated than it is.)

If you haven't attempted Content Center editing before, you first need to add your own library (all the supplied libraries are read only for good reason!) - copy the structural shapes you want over to your own library - and then you can start editing. 

[xenocatalyst]

I've already set up a few custom libraries myself.

The inventor content centre has a few gaps when it comes to the Australian Standards.

Flat bar is one of those I've had to make. Structural bolts is another one.

I find it both interesting and frustrating.

Sometimes, meeting the engineering requirements requires using sizes that are not available as flat bar and that is what let me to this question.

Thanks for the input. No doubt I'll have more questions.

[pcrawley]

I'm also using the Australian Standards (most of which come from JIS anyway).  The Aussie standards are included in the library called "Other" - you won't find them in ISO or ANSI.  The Aussie content - particularly steel section sizes did get a big update a couple of years ago - thank you Autodesk.  But as you say, finding the right sizes can be frustrating which is why I spent some time culling the stuff we can't buy and adding the non-standard sizes we can.  It was a couple of days of effort that I've never regretted. 

That said, I didn't make the Flat shown, I copied it from an existing library.  I'll see if I can find it again to save you the extra work.

[xenocatalyst]

Thanks for the offer Peter, but don't trouble yourself, I've already made a library.

Roy.

[cadman777]

I've done this with holes and a few notches in a medium sized structure.

Granted I did it in an older version of Inventor.

After about 10 holes, and 2 notches, Inventor began to do strange things.
And when I edited the master sketch so that things moved a little bit but nothing changed (the whole model locked up), all the notches broke, some of the holes broke, and it was impossible to fix them without starting over. Man was I pissed! That happened more than once, so I quit using this method.

I GIVE THIS METHOD A GIGANTIC THUMBS-DOWN FOR STRUCTURAL CONNECTIONS!

There really isn't a reliable and cost effective method for using Inventor to do this, unless you create a library of connections which takes an unbelievable amount of time, planning and coding.

If you want a cost effective structural app that does most things pretty good, check out ParaBuild.

[pcrawley]

@cadman777 - Good point!  Both copy object & sculpt methods can easily introduce adaptivity - and adaptivity in FG assemblies is almost always bad.

With large FG assemblies it is often tempting to project geometry from a frame member back onto the layout sketch.  It is also tempting to project geometry between frame members.  But this sets up cyclic

As soon as you see the adaptivity symbol in the browser in an FG assembly, you know there will be trouble ahead.  If you can't resist using project/sculpt/copy object, hold the CTRL key while project geometry or deselect the adaptivity option in the feature creation so stuff isn't adaptive and accept that it will not update as things move.  Even better is to make edits to your layout sketch(s) by opening the part in its own window.

[cadman777]

@pcrawley " hold the CTRL key while project geometry or deselect the adaptivity option in the feature creation so stuff isn't adaptive and accept that it will not update as things move.  Even better is to make edits to your layout sketch(s) by opening the part in its own window."

Yeah, I've done all that in the past. The next-best method I found is using AssemblyFeatures. But they add a level of complexity to the FG model. The best method I found is to use a MasterSketch for everything, even hole locations. The master sketch can be used with assembly features in the FG model too. You just need to use WorkPoints to locate the holes and other features. All of it SUCKS for structural connections b/c it's a round-and-round-we-go-and-where-she-stops-nobody-knows scenario if the model changes and updates occur (like you said).

This subject has been hashed and rehashed many times in this forum. There's a long thread somewhere by I forget who that talks all about this.

[blandb]

I agree with you, it was just a quick idea based on the info given. I wasn't sure how much of the structure was completed, and having the user go and publish and re-do a bunch for the design, it was just a isolated solution for the specific scenario. In the grand scheme of things, definitely would be ideal to publish plates and use the actual notch command. Or, as others and you have mentioned, use Tekla or some structural software.

One thing to note is, Inventor doesn't produce structural detail drawings like SDS or Tekla, etc. The AISC standard is different than what INV spits out. I worked for a structural company who was trying to utilized INV in a structural world expecting to spit out their standard of drawings, and it wasn't working. So, a user is needing to follow that standard, it will be difficult.

[cadman777]

I get it. It all boils down to the level of experience the user has combined with 'git-er-done'.

Far as Inventor not being able to ISO, AISC, etc. structural drawing standards, I think that can be remedied with VB.Net. But who wants to pay a coder the zillions of bux needed to make such an app when you can spend $6k once (ParaBuild) and be done with it? Besides that, all the jobs I did were small so basic drafting was all that was needed to get the job detailed. I actually have the 1983 version of 'Detailing for Steel Construction' by AISC which I used in the past for bigger structural jobs. The way they detail trusses leaves a lot to be desired! Anyway, I guess the key here is getting 'the right tool for the right job' or 'winging it'.

[xenocatalyst]

Oops, Looks like I opened a can of worms.

[pcrawley]

Haha - but it was can of well-meaning worms! (Although it is sometimes frustrating to see second-hand non-specific opinion presented as a reason for you to not try something.)

Only you know what you are planning to do with Inventor.  It looks like structural steel work, but my granny always said "Don't judge a book by it's cover" - and that's exactly what we've all done (including me). 

Good luck with your project - and if it is done in FG and you have more questions, I hope you return here because there are a lot of great contributors happy to help.

[AIR_123]

@pcrawley @cadman777 
I absolutely agree with you guys! In my opinion IV should not be used for that...

Such parametric "incompatibility" of FG is absolutely devastating in production environment. 

[xenocatalyst]

Well, I'll get your opinion then. 

Would you use IV FG to produce GA and Shop detail drawings for a structure like this?

[cadman777]

I would definitely NOT use Inventor.

I'd use ParaBuild or something similar.

It's all about:

1. the grid

2. connections

3. automated assembly drawings

4. automated weldment drawings

5. automated single part detail drawings

6. automated BOMs and other types of lists

Inventor can't do any of that.

Inventor is a boat anchor for structural work.

Nice looking framework!

Incidentally, I would shy away from both Tekla and AdvanceSteel.
It's a matter of price-point for me.

Tekla is extremely expensive and has a steep learning curve.

AS is a lotta money for a mid-range structural app and I assume it too has a steep leaning curve.

I've used Tekla's educational version and ParaBuild's trial.

Learning curve on Parabuild is mild in comparison.

It can do pretty much all the basics.

If I had a lotta structurla work, I'd buy it.

But the Tekla guys have beat me out b/c it's all automated on CNC lines.

And the ONLY thing they use it Tekla data.

So nothing else can compete around here.

Pretty sad the way the corporate mafia took total control of the industry where I live.