Help with sheet metal chute design

[ak-thermovac]

Hey everyone.  I asked for help with a similar part about 2 weeks ago and the feedback that I got was extremely helpful.  I was able to complete my first sheet metal fabrication (almost) entirely in Inventor.  I say "almost" because on the previous post, I had started out with a wireframe that I developed in AutoCAD, and imported into Inventor for conversion into a sheet metal fabrication.  This time, I would like to get some ideas on the best way to go about modeling the attached chute (customer supplied 2D drawing, to scale), as a sheet metal part, ENTIRELY in Inventor.  I need help getting started, because I don't know the best, or even a good, process for developing this shape, or the wireframe thereof in Inventor.  Once I have the wireframe, or sketches of the facets, I will be good to go.

I started down the path of creating work planes for each face, and sketching on those workplanes, but that seems terribly inefficient.  I have to believe there's a better way.  If someone would take a few minutes to help, I would be very grateful.  No need to make the exact shape as shown in the attachment, but something similar, so I can get an idea of how to do it.

I've also attached a jpg of the completed project that I asked for help with last week (referenced above) in case anyone is interested.  It's a material handling chute with bolt in liner panels on the sliding surfaces.  It's my first sheetmetal project, and it went way better that I had expected.  Hopefully the fab department thinks so too.

Thanks in advance!

[cadman777]

I've done plenty of chutes with liners over the years and found the only way to do them so they can update down the line when changes occur is by creating 2d sketches on workplanes like you are doing. The key is to make sure all the connecting points that the adjacent sketches share update w/the changes to the previous sketch.

My normal method is to create a master sketch and Derive it into each sheetmetal part and include only the necessary sketches. Then use normal sheetmetal commands to make the part and flatten it.

One challenge is to try to make the sketches are 'lean' as possible. If I'm starting from existing machinery that can be tough. But if making my own from scratch, that can be good b/c you can make everything as symmetrical as possible, which cuts down on the sketches and geometry.

I always make the sketches for fasteners art the very end of the master sketch b/c they can be quite involved if not. Sometimes a 3d sketch or two may be needed. But I try to not use them if possible b/c the geometry has a tendency to get skewed when things change upline.

Also, I've Derived the shell into a sheetmetal part for creating the liners. you just use it as a work surface b/c all the holes are already in it. You just delete the edges and back face and Thicken it to the desired thickness. Then you can countersink the existing holes or do whatever you want to them, but make sure you Derived into that sheetmetal sketch the hole pattern Parameters so you can make one CS and then pattern the rest. 

That should get you started.

Let me know if you have any questions...

Incidentally, nice previous chute!

[JDMather]

Can you Attach the *.ipt file of your attempt here?

[JDMather]

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@cadman777 wrote:

... creating 2d sketches on workplanes like you are doing.

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I prefer to create a master surface body and sketch on that rather than creating workplanes.

https://www.youtube.com/watch?v=8wo9MB-QtAQ&list=PLp5izJt_zvN2xrvzLOIsHWjQ6mbtQXLN1&index=15

[cadman777]

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@JDMather wrote:

I prefer to create a master surface body and sketch on that rather than creating workplanes.

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Seems like a lotta people in here do it your way.

Only reason why I do it the workplane way is b/c all of what I do are retrofits that are either laser scanned or hand measured. So that means none of the sides are orthographic. Sometimes the compound angles are really strange. But sometimes when I get the scan, someone's already consolidated it down to only what I need, and it'll end up being a bunch of surfaces like you use!

[ak-thermovac]

Thanks for the input so far guys... I've already left the office for the day, so I can't attach the ipt right now.  Unfortunately, I got a little way down the path of creating individual work planes and then sketching on those planes, when I decided to undo a lot of what I had done because I thought of a way that might work better... turns out I wasn't as clever as I had thought.  When I get back in the office tomorrow, I'll open up the pyramid hopper attachment and see what I can gather from that.  I really appreciate the help.

Incidentally, this project is in fact a set of laser scanned retro-fit chutes.  The CAD file that I attached was an original from 2012, but we also have the point-cloud data for this chute as well.

Again, I really appreciate the help.  I'm very tempted to fall back on AutoCAD to make the wireframe, just because that's what I know, but I really want to learn how to do it with inventor too, because I think it might be more efficient once it clicks.

Also, you got another subscriber JD!  Thanks!

[cadman777]

My advice as a former AutoCAD user of many years:
Do it in Inventor.

Take the time to learn a process that works for you.

You will never regret it!

[JDMather]

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@ak-thermovac wrote:

I'll open up the pyramid hopper attachment and see what I can gather from that. 

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I got lazy and cheated on the reinforcement bands and didn't use Sheet Metal or Frame Generator as separate components.  I should have added a bit of clearance for the side pipe too.

[ak-thermovac]

Thanks guys!  You helped over another learning bump.  I actually used a combination of methods from both of you.  The key for me (referencing the attached file) was getting sketch 3 and sketch 6 set up and extruding them as surfaces, similar to how JD set up his hopper. After extruding sketch 3, I used the resulting surface as the termination for the extrusion of sketch 6.  This gave me the back, sliding surface.  Making the corner panels was a challenge.  I used cadman777's advice and went with workplanes and sketches.  After that, the sides panels were easy.  

Feel free to critique my method.  I'd love to learn how this could have been done better or easier.

Thanks again!!

[cadman777]

Glad you figured out a work-flow.

One thing I forgot to mention is, unless impossible, I always put my sketches on the inside surfaces so they thicken outwards. That way the corner-to-corner welds are natural, or the formed corners are also easier to accomplish. You can join adjacent sheetmetal corners with bends by just thickening them one at a time (you may already know that).

Sometimes my sketches look a little 'busy' due to compensating from working from the inside surfaces. But in the end, I never have problems with updates when things change or the model needs tweaking. I can't view your part file b/c it's too new for my version of Inventor, but if I have time tomorrow I'll post an example of my method of MasterSketch driven parts.

[ak-thermovac]

Yep, I realized quickly that sketching on (what will be) the inside surfaces seems to be the optimal way to go for this type of work.

I had been working with Inventor 2020 up until yesterday, when I was finally forced to update in order to have a look at JD's hopper file.  Now I'm on 2022.

Anyway, I really appreciate your assistance.  This is so much more efficient that designing and then manually developing flat patterns in AutoCAD.

[cadman777]

Great.

I also do tanks that way, working them from the i.s. out.

Pretty much any thin walled vessel can be done like that.

There are some exceptions, but I can't think of them at the moment...

[cadman777]

Here's a quick example of the way I would do it.

Basically, I work back and forth between the MasterSketch and the parts to build the whole weldment or assembly.

Start with the known and work towards all of the unknowns.