Structural Steel sections

[MikeKovacik4928]

Hi All

I am very rarely on here now, only when I am doing after hour freelance work with my personal licensed copy of Inventor Pro 2018, like now. My full time job is now managerial, running a drawing office of 5 draughtsman all using solid edge, which I am very slowly trying to learn.

With steel sections I have created a library over the years of the steel sections, drawn according to dimensions from the Southern African Steel Construction Handbook. This library has just been one metre long sections, ipt's, saved to my own library in my own specific location.

When I need it I take the ipt for the specific section and do a save copy as to where I need it, then adjust the length and add all the cutout, drilled, mitred etc features.

This has proved simple and effective and nothing has ever gone wrong.

I have never used frame design or ifeatures or iparts.

I have experimented with iparts, I have thought about ifeatures, and I have steered clear of frame design.

In a design where you have done a frame using a certain steel section, lets say a BS taper flange channel

(BS 4 : Part 1 : 1993) like C200 x 75, and then want to change that whole frame to say C180 x 70 I could see the 

advantage of using some thing like ifeatures where you could change the whole frame quickly without remodelling,

by just going into the sketch and changing the ifeature? Not exactly sure how this would work, would have to experiment with it.

How do you guys out there do it? What have you found to be the advantages and disagdvantages of your methods?

Mike Kovacik

Inventor Pro 2018

South Africa

[MikeKovacik4928]

okay 

here is how I usually draw my steel sections.

from here I will extrude and then experiment with making Ifeatures of other channel sections.

Mike Kovacik

Inventor Pro 2018

South Africa

[Frederick_Law]

Did you check if Frame Gen got the same structure?

In Canada, CSA is the same as ANSI.  Only size shown in metric.

So I just copy ANSI and change the name.

[MikeKovacik4928]

Thanks

The frame generator has the same structure, but it seems as if frame generators dimensions are different to the South African Steel construction hand books dimensions for the same standard BS4. 

So I will stick to my method, it is simpler, doesn't take long and has never failed me yet.

Mike

[dave.cutting]

Hi,

You could create a copy of the section that you want.

If you then create a part using this new library and save it with a filename of your choosing outside the content centre folder you can modify it to your required dimensions.

If you then go back to the content centre family that you created earlier you replace that families template with the file that you created earlier. All of that family should then use your South African standard.

[Frederick_Law]

Since you're asking about iFeature.  You are looking for change and improvement.

Frame Gen will be a step above iFeature.

You can mix and switch different structure in Frame Gen: C, L, Pipe, Tube.

iFeature only let you change size.

Try Frame Gen with Content Center profiles.

You can add your standard after if you like it.

[MikeKovacik4928]

Thanks Guys

I will continue for the time being doing, in my current project, what I have been  doing, but will definitely look at content centre, and frame generator and how they work and try to use for future projects.

I will also look at ifeatures in the future just to figure out how it works. I might find a use for that too.

Mike Kovacik

Inventor Pro 2018

South Africa

[Frederick_Law]

Structure is more on iParts and Model State.

[CGBenner]

@MikeKovacik4928 

Hi, Mike.  It's not my job to try to sell anyone on one workflow over another, but since you asked how we liked to do things, I'll just tell you my experience from when I was designing frames all the time before I came to Autodesk.

In the first few years of my old job, our company used iFeatures like you are doing for all of the frames.  It worked, but we found it to be harder to make changes because of the way everything was constrained.  Not impossible... just more challenging.  We left Inventor for a few years and tried ProE (WF4 &5) and used their frame design module.  During that time, we got used to the robustness of the sketch-driven design style.  When we moved back to Inventor (for many reasons), we tried Frame Generator and found that it was even better than the ProE equivalent for what we were designing.  It did take a while to create some custom libraries for some of our sections, though most were readily available as standard ANSI sizes.

So,... bottom line, my opinion is that you would be happier in the long run by taking the time to use the tools in Frame Generator.  But it's just an opinion.  Good luck in whatever you do.  🙂

[MikeKovacik4928]

Thank you for sharing your valuable experience with me Chris.

I will definitely take that into account going forward, and in my main daytime job,

where I am very slowly learning solid edge, will also see what the solid edge equivalent is.

Mike

[chris]

@MikeKovacik4928  I use a robust set of iLogic structural steel members I created, complete with copes, chamfers, etc, the beams and channels also have plate profile support. Frame Generator has some advantages, but it seems silly to create (2) assemblies and a part sketch to place a single piece of structural member. I think most people use the FG for the cope and finish aspects, I just find it easier to use user created structural member templates so I can have the assembly talk to the parts and control everything at the top level (just my 2 cents)

[CGBenner]

[Non-serious response]

While I would NEVER advocate violence against animals, this thread is a perfect example of the old adage: "There is more than one way to skin a cat."  🤣🤣

[cadman777]

Mike,

I have used the ContentCenter for over a decade. But first I made my own profiles, b/c the out-of-the-box Inventor profiles suck. They are mirrored halves of each section, which makes it impossible to modify them in any meaningful way. Plus, they have way too many Sketch constraints due to the mirroring. So, I not only simplified the profiles, but I also added a Gauge line where the bolts are supposed to go, as well as adding other info to suit my design venue.

The two biggest changes I made which brought the greatest benefit is that I combined all I-beams into one CC part, all Channels into one CC part, all Angles into one CC part, etc. And, I made all the Parameter names uniform across all CC parts, including Pipes, Fasteners, etc. The benefit of that is that the BOM can be easily structured and sorted, which means the drawing Parts List self-populates every time (for about 95% of the parts).

So when a particular profile already exists in a model, and then it needs to change type and size, I don't have to start all over again with all the modifications made to it. I just RMB on the CC part and pick the size I want and all the holes, cuts, etc. repopulate the new CC part. Angles is a good example. Autodesk, in their infinite wisdom, split them into Equal vs. Unequal leg length, so you have 2 different parts in the CC for one structural shape. Wasted work time is why I combined them all into one CC part file, b/c every time I needed to change the leg type (Equal vs. Unequal) during a design, I lost all that work I did on the Equal leg Angle and had to re-do all that work on an Unequal leg Angle! So, after I had my CC all setup, it was easy to use any CC part any time I needed it. 

Here are some examples of how this works well for me:

1. Place an aluminum ANSI Channel in a machine frame, make all the copes, holes, pockets and cuts. Then later in the design it needs to change to Architectural Channel. So I simple RMB on the part and pick it from the list. No fuss no mess.

2. Make a Master Sketch framework for a structure. Place a steel ANSI W-bean into the weldment assembly @ 0,0,0 World, Grounded. Then open that part file and Derive the Master Sketch into it. Then locate the Sketch line where that beam goes, and modify the part so the sketch and Start/End planes are on that 'wire'. Make all the copes and holes, and then close the part. Open the assembly and it's in the correct position with all the trimmings. Then later in the design if it needs to change size, I simple RMB on the part and pick it from the CC list and the profile updates. The best part is, when I need another beam of that same profile, I just copy the file and rename it, then place it into the assembly @0,0,0. Then open it and change the placement of the sketch and Start/End planes. If the copes or holes need to change, it's much easier than starting from scratch.

3. I need a profile for a curved beam. Since I know my CC parts have nice clean simple profiles (not the junk that comes with Inventor), I delete the Extrusion and re-work the part on an arc or sketch with arcs and lines.

4. In a fully welded structure with many members, I use a Master Sketch with profiles converted into Blocks. That's the quickest way I found to re-use CC profiles in a Master Sketch if I want to put them all into one sketch. To make each part, I open a new Part and Derive that Master Sketch into it, then add Start/End Work Planes, and make a From/To extrusion, add holes, cuts, etc. Then place that part at 0,0,0 World in the weldment assembly file. The main draw-back to this method is it populates the Parameters d/b with a zillion Parameters, one set for each Block. So the Parameters d/b can get a bit crowded using Blocks.

5. The benefit when making a structure using Frame Generator is that all the parts will have uniform Parameters and iProperties for the BOM and Parts List. BUT, making copes and holes is a mega PITA due to their non-inclusion in the part file for when making drawing details of each part.

Note: I always use Custom CC parts instead of defaulting them into the Inventor 'Library', b/c the library part's iProperties can't be changed in the BOM.

6. The way I made my CC parts according to ANSI standards is, someone in here posted a link to the ANSI web site where they provided an official Excel spreadsheet of all their profiles, both modern and legacy. So I downloaded that ss and created one good profile for each structural shape. Then Authored each shape with all the relevant Parameters and iProperties in it. Then I copied the ANSI ss and separated each profile into a separate sheet in the Excel file. Then re-arranged the columns to match the order in my CC part Family Table. Then I opened the Family Table in Excel and copy-and-pasted all the data from the ANSI ss to the CC ss. Then I tested the new CC part and made the necessary scrubs to it. That whole process took about a week to accomplish. It has served me well over the years. IMHO, this is what Autodesk should have done from day-1. Simple is always better in engineering and design.

Let me add one thing about creating my own CC profiles. When you dimension them, be sure to rotate them at a slight angle. That way when you place the dimensions, you can be sure they're Aligned with the Sketch entity. When finished placing all dims, you can reorient the entire Sketch using a Vertical or Horizontal constraint so it's back to 'true'. The reason you want to do that is when you re-use the profile and need to rotate it. If you don't do it that way, then when you try to rotate the profile in the Sketch, you get stuck b/c some dimensions have defaulted to Orthographic. That means you will be forced to delete all the Ortho dims and remake them. That ruins your CC profile, due to all the connections it may have in the Parameters and iProperties. In retrospect, that's one thing I didn't do that I should have done when making my own CC parts.

[cadman777]

@chris,

I'm curious how you do that simply so you can include all the possible combinations of copes between any kind of beam each end may encounter, including the gaps and all of that? That's where I got stuck trying to accomplish that feat, since there's a myriad of potential cope combinations, depending on T/O beam to T/O beam and beam-to-beam combinations, including cross-beams positioned at angles to running beams.

[chris]

@cadman777 I took the time to setup cuts for angle, channel, beam etc, then I have those mapped to a parameter True/False to make suppressed or active and within each cut is also the choose to choose the beam, angle or channel size. I'm not saying it's perfect nor is a small part file, but it does work. (Just don't make event triggers for it that are set to open or close part), for some reason it dirty's the part file and you'll be constantly checking in/out

Here's an example 

[cadman777]

That's really slick!

I like the GUI.

So for your copes, do you access an Excel file that lists all the structural shapes and sizes?

Or are they embedded in each shape's template file?

If so, doesn't that bog down the system when you make elaborate structures?

[chris]

@cadman777  The above example is logic and ref'd an excel sheet, the newer version is in iLogic only, I suppose if you were running a scrapper it might bog it down, at most I've only had these in assemblies with a couple hundred structure members. I'm sure it could be made more efficient, my iLogic skills are very basic

[chris]

@cadman777 I can add a couple of them up later and ya'll can play around with them or improve them

[cadman777]

Excellent.
Thanx!

[chris]

@cadman777  Here are a couple to get you started, some are old iParts, some have embedded excel that iLogic references and some have everything in iLogic