Archive for the ‘Sheet Metal’ Category
December 16th, 2008 | 
Author: I stayed up late last night watching a long collection of sheet metal related videos. Some were tutorials on how to bend metal by hand or with simple tools, with a hammer, a leaf brake or a box and pan brake; some others dealt with the design of tools and dies. I know this doesn’t replace visiting a real shop and (hopefully) getting a try at bending a piece of metal myself, but the videos were extremely detailed, with lots of close up views, and at least I got to see different kinds of presses in action. This one is one of my favorite ones. Just wanted to share with you here, for those that, like me, had never seen one this before.
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One thing I’m learning quickly about Sheet Metal product design is that coming up with a sheet metal part or assembly in SolidWorks (or even a hand-drawn pattern for that matter) is only the first part of the story. The interesting part is now figuring out how it is going to be fabricated! This means that, besides a pattern, we also need to come up with a sequence of operations that takes into account the kind of tools or equipment we have at hand. Jeff Cox has some very interesting thoughts about it in his blog. Check it out! It’s really an eye opener for those of us that are just learning.
And now, let me tell you a bit about the sequence for fabricating that little tote tray I told you about in a previous post. Take into account that all that’s available is a small leaf press and some hand tools, like shears, hammers, a pop-rivet gun, etc. Not really a big shop… but still good enough to learn!
Anyway, once the stock has been cut out to size according to the pattern, the question that comes to mind is “What do we bend first?” I was under the impression that we simply had to do it in the same order as the flanges and hems were added to the part in SolidWorks, but it turned out to be quite the opposite. In my SolidWorks model, for instance, the hems are the last thing to be added, but as it turns out, hems should be the first thing to do, since it would be very difficult to fold them after the sides of the tray are bent up. Also, we are supposed to look for ways to make several operations at the same time, rather than one by one, to make it more economical. There are also operations that won’t be possible with the kind of equipment at hand. I was told we can bend the sides using the leaf press, but not the ends of the tray; those will have to be bent by hand. We could bend them if we had a press brake, although I’m not exactly sure what the difference is, and why the press brake could do it while the leaf brake can’t. I sure would love to see a press brake in action! This is a fascinating area that I wish I could learn more about!
Back to the example… It is possible to convey information about the sequence of operations to bend your part simply by creating a few configurations and suppressing a few bends. Here is how. In the feature manager, locate the feature Flat Pattern. This is usually suppressed when the sheet metal part is folded. Click on it to expand it and you’ll see a list of all the bends in the part.
Create a new configuration for the part and name it Flat, make this configuration active and unsuppress Flat Pattern. This will be our starting point.
Next, we need to create a new configuration and name it STEP1. We can simply make a copy of FLAT, since most of the model will be flattened, except for a few of the bends. In the Feature Manager, we expand Flat Pattern (which should be unsuppressed in this configuration) and look for the bends that correspond to the hems in the part to suppress them. This can be a little tricky when you have bends that have been mirrored.
Now we need a new configuration for the following step in the sequence, STEP2. The easiest way is to make a copy of STEP1, since we’ll just continue suppressing more of the bends in the list, in addition to those we already suppressed. For STEP2, and according to the pattern I had originally, we should find and suppress the bends for the sides and tabs, so they could be folded together in one operation. However, I wonder if the sides and tabs can really be folded in one operation, because the bend is not exactly located on the same line for both. See?
Assuming they could really be folded together, this is how STEP2 would look like after suppressing the bends.
The last step is to bend up the sides, which leads us back to the default configuration of this sheet metal part, which I’ve renamed FOLDED.
Like I said before, I think Sheet Metal design is very interesting and I really want to learn, so I would appreciate if those out there reading this that may have more experience than I do would take some time to explain how they would approach the sequence of steps for the tabs and sides… one step for both? Two steps? Which one would go first? Your advice and expertise is always welcome and greatly appreciated!
Unlike others, I was never introduced to sheet metal forming techniques while in high school or even in college. There was a class we all were required to take on manufacturing processes, where it was briefly discussed, and we also had a shop were we learned to use a few tools and machines, like the lathe, as well as several welding methods. I used to cut and prepare metal for welding, but I can honestly say I never learned how to bend it and form it. I’ve bent tubes in the past, though if that accounts for anything…
Anyway, I’ve been curious about sheet metal, so I’ve been doing some research and, with a little bit of help from here and there, learning about basic techniques with a small leaf brake. One of the beginner’s projects is a tote tray. The pattern seemed really simple, so I thought I would try and model it in SolidWorks. It was certainly a good exercise, and not as simple as I thought.
The tote tray is an assembly of two parts, the main body of the tote tray and a handle, as you can see in the following image.
I started modeling the main body by first creating a rectangular base flange. The pattern called for 24 gauge metal. I assumed it should’ve been galvanized steel, but I only have a couple of tables that come with SolidWorks, and the only 24 gauge metal available was Aluminum, so I used that one. Once I had my rectangular flange, which is actually the bottom of the tote tray, I proceeded to add an edge-flange on one of the short sides. To do this simply select the edge and click on Edge-Flange on the Sheet Metal toolbar. You will see the Edge-Flange property manager on the left and a preview on the graphics area.
The arrows you see in the preview allow you to modify the direction of the bend to go up or down. You can also modify the angle of the bend through the property manager. I need an angle of 90°. I’d also like to mention something else that you can’t appreciate from this image: when you first add an edge flange to your part, the shape of the flange is going to be rectangular, just running all along the edge. The reason why my edge-flange looks different is because I modified the sketch used as the flange profile. It’s not hard to do, just click on Edit Flange Profile in the property manager, modify the sketch and then click on Finish in that little dialog box, as long as it says that your sketch is valid, of course.
Next, and still following the pattern, I added a hem to two of the edges. From the property manager, I chose a closed hem and material inside option. Unlike with the edge flange, it does make a difference which edge we choose for the hem. If I had chosen an edge on the outside face of the flange, then the hem would’ve been added to the other side.
After mirroring the first edge flange and its hems, I added another edge flange to one of the sides and then a third smaller one that the pattern calls for and that, I believe, will help close the box. My choices for this one had to be slightly different than for the rest, to accommodate for the material in other parts of the box. The pattern I had didn’t mention this. Anyway, for this flange I had to choose to have the bend outside, since choosing material inside or even material outside would cause interference with the other parts of the box. You can appreciate in the image that there is a small gap between this flange and the second one I made on the side previously.
The rest of the flanges and hems were made in a similar fashion, I mirrored whatever operation could be mirrored and then trimmed the corners.
I had a pattern for the handle of the tote tray, as well, so I first tried to make the part and assemble both together, but it wouldn’t fit right; there was a lot of interference between the two parts. So, I decided to try modeling the handle in context. For this purpose, I added a plane to Tote Tray 1 (the main body of the tote tray), where the bottom of the handle would be placed. The first thing I noticed was that I needed to find a way for the sides of the handle to clear the hems of the first part, so while sketching the flange for the bottom of the handle, I left a gap big enough to make sure there would not be any interference (the thickness of the metal plus a little bit more to allow for the gap in the bend of the hem). This can be better appreciated in the following image. Notice how the hem passes behind the flange and both parts don’t interfere with each other no more.
A similar consideration needed to be made for adding what the pattern calls a “hook” for attaching the handle to the main body of the tote tray. I did this with another hem, choosing for it to be open, with the bend outside and a gap distance big enough to clear the gap I had left in the beginning, when sketching the bottom flange, plus the thickness of the metal, as you can see in the image.
Once again, I added a couple more flanges to the sides and mirrored whatever could be mirrored to obtain the final result.
I don’t know if this is the right or even conventional way to do design in sheet metal. When I unfold the parts, they look pretty much like the pattern I had, but the measures just don’t quite match, because mine takes into account all those issues with interference that seemed ignored in that other pattern. It’s almost as if the other pattern assumed that the bends wouldn’t take space at all. Hmmm…
This part is an IGES file that is included in the SolidWorks 2007 Sheet Metal Training Manual as one of the examples on how to convert an imported (dumb) part to sheet metal.
According to the explanations in the manual, this can be done as a two step process, by first using the Rip feature to select edges or corners that will be cut with a small gap in order to allow the part to be flattened as a sheet metal part, and then adding bends using the Insert Bends feature. Or it can be done in only one step, selecting Insert Bends to recognize the bends in the part and rip corners at the same time. In this image, Face 1, the fixed face, is the bottom rectangular face of the part, the edges highlighted in blue are those that will be ripped, and are listed under Rip Parameters, together with the gap value of 0.5 mm. Other options are also available, such as changing the bending radio or auto relief.
The result is a sheet metal part, with rips and bends that have been added to it and that we can select and edit separately through the feature manager. Notice that the sharp corners in the original part were converted into sharp bends using the default bend radius value, while the existing bends, like that tab on the right, were converted into round bends, using their current radii.
The flattened sheet metal part looks like this.
So I tried doing the same using the new SW2009 feature, Convert to Sheet metal, but I’m afraid my results were not all that good.
I tried making similar choices to those I made before, in order to achieve the same results. For the fixed face, I chose the same as before, the bottom rectangular face. Hard as I tried, SW would not allow me to choose the edges to be ripped in this case, so I chose the edges that represented bends instead (in pink), and SW identified the edges to be ripped (in purple). I chose the same bending radio and the same gap as before.
At this point, everything seemed to be going exactly the same as when using Insert Bends, but then I noticed something. It’s kind of hard to see while looking at the isometric view, because the part is made semi-transparent, but notice how, as you choose your edges, a preview of what your converted sheet metal part will look like appears on the screen, in a yellowish color. Notice that everything in the part seems to be included already, except for one thing: that little tab on the right. Can you see it? The tab is not colored yellow like the rest of the part, which means it will not be included in the sheet metal part.
Why is this? Well, I think the bend hasn’t been recognized. So, I tried the button that says Collect All Bends, but got a message saying that no previous bends had been made. I also tried selecting the edge in the part, but got a message saying that this could not be a bend edge since there was a face for this edge that is not planar. So, without any more ideas on how to make SW recognize this bend, this is what results from using the new SW2009 feature on this particular IGES file. The tab is gone and we only have sharp bend features added to the feature manager, but no round bends like in the previous example.
So, I guess the new feature isn’t really the tool to use for these particular kinds of parts. I do wish there were a few more examples of the uses and limitations of the SW2009 Convert to Sheet Metal feature, especially for those of us that are just learning about sheet metal altogether.
So there I was, seating in a meeting room with my older son’s SLP, his two teachers and the principal. We were discussing what his progress in speech therapy had been so far, and what other areas of concern would be addressed this year. One of the teachers then proceeded to describe my son’s behavior in class and what she considered a source of potential trouble. “The boy seems a little too fidgety”, she said, “I can never be sure if he’s paying attention or not, because he’s always doing something, like playing with the pencil, rocking in his chair, etc. Do you have any idea what may be going on with him?” OK… At this point I had to force myself to stop wiggling in my chair and quickly hide all the origami I had been making out of the papers I was given by the SLP when I arrived. Phew, that was a close one!
Don’t take me wrong, I really was paying attention during that meeting, but I also have to admit that this behavior of his is probably learned, and that it’s not hard for me to get distracted like he does. One of my biggest distractions is the internet. It’s so easy to get lost in it! You start by reading one of your favorite blogs, then link to the next one, catch up with the latest gossip at the forums or Twitter… Before you realize, you’ve already spent there a good thirty minutes or more! That’s why I’m making a covenant with myself to stay away from it (especially from things like Twitter) as much as I can. I will still read my favorite blogs and check what’s new on the forums, even on Twitter, just not so often. So far, the plan is working, and I managed to get a lot done just this weekend.
Fellow blogger Brian’s announcement of his big success with the Sheet Metal test made me curious, and so, among other things, this weekend I took a look at the Sheet Metal tools available in SolidWorks. It doesn’t seem as hard as I thought it would be! While I don’t know much about sheet metal outside of SolidWorks (and I would really like to learn), I managed to use a few of the sheet metal features to model a common household item, this cheese grater. I saw this one in a magazine, the one I own is actually flat. If you look for a cheese grater online you’ll probably find dozens of different styles and sizes.
So, anyway, the fun was in making the “grater” part, because the handle was made with a sweep boss and a couple of extrusions, so nothing new there. Here is what I used the sheet metal features for. I started by sketching a rectangle centered at the origin, then using Base Flange from the Sheet Metal Tools to create the base feature of my sheet metal part. As you can see, it looks a lot like a common extrude boss, but by using Base Flange instead of Extrude Boss, I’ll be able to use other sheet metal tools on it that otherwise would not be available to me.
Next step was using Hem to curl two of the edges of the sheet metal flange, to simulate the way in which the edges of the “grater part” wrap around the handle’s wire frame. The rolled kind of hem worked the best for my purpose. I specified a radius and an angle big enough for the hem to wrap around as much as possible, without touching the rest of the flange.
Next stop was creating my own forming tool. A forming tool is what you use to make any kind of dent on the flat sheet metal part. The dents you create this way have the same thickness as the rest of the part. SolidWorks provides a few in the design library, but you can easily make your own. I started by creating a part with the basic shape I wanted to punch on my cheese grater, and then transformed this part into a forming tool by using Form Tool from the Sheet Metal toolbar. The face in green is the Stopping Face, this one corresponds to the face to which you apply the forming tool. You need to have a stopping face when creating a forming tool, that’s why I modeled the shape of mine using a "plate" base. The face in pink is the one that will be removed from the sheet metal part when the dent is made. The direction of travel of the tool is always going to be normal to the stopping face, so it’s important to give some thought to how you want the dent to look like. When you’re done, save the part as a forming tool (*.sldftp). You can add it to the other forming tools in the design library or create a separate folder to keep all the forming tools you are using for your project.
To use this forming tool in a sheet metal part, you simply drag it and drop it, then rotate and position the orientation sketch as needed.
The next step was patterning the dent I just made with the forming tool. By the way, I know, I could’ve used just one pattern for both instances of the forming tool, but well, it will have to be next time.
I tried bending the part using sheet metal features, but that didn’t work out well with the dents I had just made to it, so I ended up using Flex to bend it slightly, taking care to position the triad correctly at the center of the part.
I must point out, though, that because I used Flex, I can’t obtain a flat pattern of this part, unless I suppress the Flex feature, but there didn’t seem to be any other way for me to bend it this way and still have the dents added to it. At least not one that I know of. If you know of a different way to do this with the sheet metal tools, please, do share! Anyway, here is the grater part as it looks finished.
OK, so perhaps this wasn’t the most conventional example of what to do with the sheet metal features, but it’s what grabbed my fancy at that moment, and it was fun too. I still have a lot to learn about sheet metal and there are things that I can’t really see a way to do with SolidWorks sheet metal tools, but I know there must be a way around. There’s always a way around…