Frame generator workflow

[Jeroen_M1990]

Hi everyone

As you can guess from the title this post is about the frame generator. At my current job I need to draw things like guards, handrails etc. And I've to use inventor due to circumstances.

So the first thing, the part numbers inventor generates are not what I, nor the workshop likes to see. So I guess the best thing to do is to copy, paste and edit in the main assembly BOM. The part number set by inventor is what I'd like to see as a description. This is nothing I can't overcome, it just makes things a bit more manual. And from what I've gathered from googling this topic, it's kind of the easier and faster solution (read little set-up time). But if it isn't feel free to shed some more light on this subject.

The other thing that really bothers me is drilling holes in frame members. The holes need to be drilled at member level, not in the assembly. I can do this quite easily if I can use the "reuse frame member" function. That way I make 1 member and reuse it across the assembly. It isn't the best function but for small assemblies and straightforward parts it works.

But now I need to design a handrail, which is divided into different sections for transport. Across these sections I use the same piece for the vertical struts, some with mounting holes and some without. The first thing I don't like is that I need to manually differentiate between one with holes and one without. Inventor doesn't recognize a difference since it generates the part number with length etc. This makes it easy to make mistakes. And to add on top of that I can't reuse the frame members either, so I've to drill the holes in each frame member separately, in every subassembly. If you try to demote members you've reused they stay grouped and all move to a single sub assembly.

So now my question is what is the correct workflow to tackle this problem? I hope my explanation is understandable.

I'm currently using inventor 2016, but I'd be happy to hear if 2017 has improvements.

[smokes2998]

Frame generator creation work flow ... It is complicated and is top down creation method...

this is the general process I have left some details out for you to figure out.

Create the .iam file save it as the top level assembly number that is not welded but has the frame in it ie a frame with adjustable feet or fasteners. ie TOPLVL12345.iam

insert a part file save it as the frame weldment number_FRAME ie 12345_FRAME.ipt as it is a reference file. ( You need to set this file to reference to stop it popping up in the bom)

Create a sketch  of the frame member  path in the inserted file ie 12345_FRAME. Note: These sketches drive the frame.

Then go back to the top level assembly you should see the sketch you have created in 12345_FRAME add a frame member to the sketch

It will then ask you to save a .iam file and .ipt file. Save the .iam file as the weldment part number ie 12345.iam  save the ipt as weldment part number_SKELETON ie 12345_SKELETON.ipt . (you need  to set this ipt file to reference to stop it popping up in the bom)

I would then open up 12345.iam convert it to a weldment file remember to set the weld material as it defaults to aluminum when requested as this will populate the material note in the drawing. i would put all the holes fro the assemble in the weld prep level of this file. 

I would then create a drawing from 12345.iam  because it is a weldment you can split out the frame members into separate views. so you can do holes as shown...

you will end up with 2 .iam files and 2 ipts files and lots frame member.ipt files.

[Curtis_W · Accepted solution]

Hi Jeroen_M1990,

If you want to push holes down to the part level use the Bolted Connection tool (just don't add the hardware).

As smokes2998, mentioned use the weldment tools to be able to detail the frame easier:

http://inventortrenches.blogspot.com/2011/03/detailing-frame-generator-weldment.html

For naming, I recommend accepting the file names, and then using the BOM editor to "massage" the part numbers, descriptions, etc, as needed:

http://inventortrenches.blogspot.com/2011/03/understanding-autodesk-inventor-frame.html

I hope this helps.
Best of luck to you in all of your Inventor pursuits,
Curtis
http://inventortrenches.blogspot.com

[graemev]

Been there, done some of that, though your needs are probably slightly different from mine.

Feel free to modify the file names as Inventor generates them. There is no particular need to accept the defaults. You can edit the Part Number and Description fields in the iProperties, too.

Reusing members is functionally identical to reusing any other part. Change one, you change all instances. If you need some to be different, "Delete Using Frame Generator" and replace with a new member: new file name, properties, and all. (Yes, it's a bit of a pain, but necessary if you're not going to use the Machining or Preparation portions of the Weldment Environment to do the holes.)

I can't speak to the BoM combining identical lengths of "different" members. If it's a problem, perhaps tweaking the skeleton to have 0.001" shorter members here and there might suffice. Inventor should then distinguish them as different enough to cause an additional line item in the BoM. (Last I checked, our shop didn't produce handrails to 3-decimal accuracy. YMMV.)

If reuse of, for example, drilled posts is somewhat rare (only occurs at "splits" of the handrails for transport considerations), perhaps push that particular post out as its own part independent of the Frame Generator and add it into the assembly manually. I can't speak to promotion/demotion of parts in an assembly, having never needed to do that, but might this help alleviate that problem, too?

[Jeroen_M1990]

Hi

First I'd like to thank everyone that has posted so far. This already gave me a better understanding, just need to try it to get it down completely. I understand top down modelling etc. it's just that I've never really used frame generator much. Nor do I, unfortunately, get any time where I'm currently working to experiment. Also I think my Google-fu might be weak, because it's all there in the blog.

Just one question though that remains. Now in my case a single frame would get pretty big and extensive. Also if it has to be split up for transport and they're to be assembled on site, what would be the best way to do that?

Would you make 1 layout and 1 big frame after which you use the demote frame member option to divide it into subassemblies? And convert those if needed into weldments. Or would you make a layout (or multiple) and create a new (weldment) assembly with a new skeleton and frame file each time? I've a feeling the latter can get pretty big. That layout will be used in each assembly that you make, and in the main assembly it might slow down the updates and saving.

Regards
Jeroen

[graemev]

---

Just one question though that remains. Now in my case a single frame would get pretty big and extensive. Also if it has to be split up for transport and they're to be assembled on site, what would be the best way to do that?

Would you make 1 layout and 1 big frame after which you use the demote frame member option to divide it into subassemblies? And convert those if needed into weldments. Or would you make a layout (or multiple) and create a new (weldment) assembly with a new skeleton and frame file each time? I've a feeling the latter can get pretty big. That layout will be used in each assembly that you make, and in the main assembly it might slow down the updates and saving.

---

I dunno about "best", but I'd be likely to use one (enormous?) skeleton repeatedly for many smaller Frame Generator Assemblies. That way if you want to make a global update, you only need to modify the one skeleton and all the assemblies will update upon opening - less risk of missing one or two along the way, or having to remember just which assemblies are affected by which modifications. Also, skeleton files are fairly "light" storage-wise.

[Curtis_W · Accepted solution]

---

@Jeroen_M1990 wrote:

Would you make 1 layout and 1 big frame after which you use the demote frame member option to divide it into subassemblies? And convert those if needed into weldments. Or would you make a layout (or multiple) and create a new (weldment) assembly with a new skeleton and frame file each time? I've a feeling the latter can get pretty big. That layout will be used in each assembly that you make, and in the main assembly it might slow down the updates and saving.

---

Hi Jeroen_M1990,

My preference is reuse the frame reference file in multiple frames. So for instance if I were creating this space ship:

http://inventortrenches.blogspot.com/2013/08/use-3d-solid-edges-for-frame-generator.html

I'd just insert that 3D solid reference file that defines the structure into each new frame-sub, and then place all of those subs into a top level when done...

or for more of a top down approach, create the top level, then create sub1, and insert the reference file, then add frame members as needed. Then create sub2, and insert the reference file, then add frame members to it as needed, and so on.

If I were doing a large number of subs, I might save off a copy of the empty sub1 with the reference file already inserted and just place a copy of it in the top level as a "template" of sorts.

Others might recommend demoting, and I have used that as well. I used the other approach before Autodesk gave use the Demote option for frames, so it might just be "old dog, old tricks" on my part?

I hope this helps.
Best of luck to you in all of your Inventor pursuits,
Curtis
http://inventortrenches.blogspot.com

[Jeroen_M1990]

Ok, got it, will see what I like the most, and use that one since there doesn't seem to be that much of a difference. Except for maybe like stated above that if you've multiple layouts you might miss something in one of them. But this doesn't have to be a problem, can also push parameters across and derrive. Only thing I guess you've to be careful of is not to create a cyclic dependency.

Thanks to everyone who helped me, this is going to be really useful.

Regards Jeroen

[smokes2998]

You can use the bolted connection tool to push details down to part level but, If you change a frame member profile or thickness the original member you are changing gets replaced with a brand spanking new part. This can break constraints and detail views. I find it  quicker to used the weld prep tools to detail the frame and if i make a change i can recover the holes quickly by redefine hole sketch plane and telling the weld prep tool to included the new member as part of the cut.