Sheet Metal Design with SOLIDWORKS
Illustration by Richard Downs

Forming across a bend


From:

Sheet Metal Design with SOLIDWORKS

with Gabriel Corbett

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Video: Forming across a bend

Forming tools can be used across bins, and in this video, we will review how to build a custom tool and use that tool to add gussets to the edge of a Sheet Metal part. Gussets are used to strengthen a bend and are fairly common in sheet metal parts. To get started, let's take a look at the few examples of what we're going to be making. In this case, here you can see we have a sheet metal bracket, we have a gusset, that's been formed into the edge of that bracket. This will strengthen this edge, and it's pretty easy to do. Let's go take a look at the tool, come down here to 6.4.tool and you can see this is the tool. This can be pushed into the edge of that sheet metal piece and actually form. That gusset.
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  1. 2m 9s
    1. Welcome
      1m 13s
    2. Using the exercise files
      56s
  2. 10m 0s
    1. Looking at sheet metal tools
      1m 35s
    2. Using and customizing the Ribbon
      2m 42s
    3. Understanding sheet metal
      5m 43s
  3. 40m 24s
    1. Creating a base feature
      5m 37s
    2. Looking at the Flange tool
      5m 12s
    3. Creating tabs
      5m 3s
    4. Making an edge flange
      5m 33s
    5. Using the Edit Flange Profile tool
      3m 12s
    6. Using the miter flange
      4m 21s
    7. Making a swept flange
      2m 59s
    8. Using the Jog feature
      5m 20s
    9. Making hems
      3m 7s
  4. 16m 6s
    1. Unfolding and folding parts
      2m 58s
    2. Making normal cuts in sheet metal
      2m 8s
    3. Adding cuts across bends
      4m 0s
    4. Making closed corners
      3m 17s
    5. Adding welded corners
      2m 18s
    6. Making a cross break
      1m 25s
  5. 20m 3s
    1. Using the Convert to Sheet Metal command
      5m 6s
    2. Adding sketched bends
      2m 31s
    3. Importing geometry
      5m 7s
    4. Looking at the rip feature
      3m 29s
    5. Creating a lofted bend
      3m 50s
  6. 17m 40s
    1. Building a chassis
      6m 9s
    2. Using the pattern tools
      3m 22s
    3. Using mirror symmetry
      2m 1s
    4. Using the split feature
      3m 7s
    5. Exporting individual parts
      3m 1s
  7. 15m 41s
    1. Using forming tools
      2m 56s
    2. Modifying a forming tool
      1m 44s
    3. Creating a custom forming tool
      3m 35s
    4. Forming across a bend
      7m 26s
  8. 18m 55s
    1. Basic assembly techniques
      5m 1s
    2. Adding cuts in context
      4m 57s
    3. Creating parts in the assembly
      5m 46s
    4. Using patterns and mirrors
      3m 11s
  9. 19m 28s
    1. Using ordinate dimensions
      4m 13s
    2. Looking at sheet options
      3m 24s
    3. Creating flat patterns
      2m 56s
    4. Saving to DXF or DWG
      3m 29s
    5. Automation with SOLIDWORKS Task Scheduler
      2m 44s
    6. Prepping for manufacturing
      2m 42s
  10. 1m 26s
    1. Next steps
      1m 26s
  11. 14m 12s
    1. Laser cutting
      1m 53s
    2. Shear
      46s
    3. Break forming
      3m 39s
    4. Turret punch press
      3m 14s
    5. Welding
      1m 2s
    6. Deburring
      1m 48s
    7. Hardware
      1m 8s
    8. Computer numerical control (CNC)
      42s

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Watch the Online Video Course Sheet Metal Design with SOLIDWORKS
2h 56m Intermediate Jul 29, 2013

Viewers: in countries Watching now:

CAD software like SOLIDWORKS makes sheet metal design quick and cost effective. This course gets you up to speed with the sheet metal tools in SOLIDWORKS for designing parts and assemblies, and then takes you on a trip to the factory floor to see the final manufactured results. First, you'll learn to create base features, flanges, and bends that add strength and connections. Then find out how to flatten parts and add holes, cuts, and corners that are manufacturing ready, and use the Convert to Sheet Metal command to convert imported geometry into native sheet metal parts. Author Gabriel Corbett also shows you how to create assemblies from multiple parts, use the Pattern and Mirrors tools to effortlessly duplicate existing work, and then document and export your designs. Finally, take a tour of a sheet metal fabrication company and learn about the machinery and processes that occur during manufacturing.

Topics include:
  • Understanding sheet metal fundamentals
  • Creating base features
  • Creating flanges and tabs
  • Making hems and corner features
  • Unfolding and folding parts
  • Adding cuts across bends
  • Adding welded corners
  • Using the Forming tools
  • Importing geometry
  • Using the Convert to Sheet Metal command
  • Making sheet metal drawings
  • Exporting DWG and DXF files for laser cutting
  • Building an assembly
  • Creating parts in an assembly
  • Creating flat patterns
  • Using in-context design techniques
  • Exporting parts
Subject:
CAD
Software:
SOLIDWORKS
Author:
Gabriel Corbett

Forming across a bend

Forming tools can be used across bins, and in this video, we will review how to build a custom tool and use that tool to add gussets to the edge of a Sheet Metal part. Gussets are used to strengthen a bend and are fairly common in sheet metal parts. To get started, let's take a look at the few examples of what we're going to be making. In this case, here you can see we have a sheet metal bracket, we have a gusset, that's been formed into the edge of that bracket. This will strengthen this edge, and it's pretty easy to do. Let's go take a look at the tool, come down here to 6.4.tool and you can see this is the tool. This can be pushed into the edge of that sheet metal piece and actually form. That gusset.

The green face or turquoise face here is the stopping face, which is going to be pushed to the bottom of the part. And then all the red faces will be removed from this tool. And what's going to remaining is everything that's in yellow will be actually pushed in to the edge of that part. Let's take a look at how to create this. Let's start with a new part. Click on OK. Start with a sketch, and let's use the right plane. Choose the line tool. Start at the origin. Come up, draw a little L shape. Okay. Lay a couple dimensions, 0.125.

And 1.25. And these dimensions don't really matter that much. But we want to get something that's close to the right size. Hold down Ctrl, select those two. Click on make equal. Same thing over here. Hold down this control. Select both of those. (SOUND) Make equal. And then go ahead and do an Extrude, (SOUND) let's do a mid-plane Extrude, (SOUND) 1 inch, 1.0. (SOUND) Okay. Next, let's choose the right plane again, start a sketch, (SOUND) use the Line tool, click on Space bar, so I'm looking normal to it. Go back to the line tool, grab this upper edge, draw a little triangle out on that inside faces.

And snap right to the origin, and let's go ahead and add a equal relationship between the two, from there to there, make those equal. And let's add a dimension on this lower line of 1 inch, 1.0. Notice everything is fully defined in black lines, (INAUDIBLE) with that, go to features, go to extrude and we want to do a mid plane extrude again and just a quarter of an inch so 0.25. Click OK.

Next we want to radius, this top edge. So, from this face to that face, to this face. And we want it to be one smooth transition. So I'm going to go up here to fill it. I'm a deselect what I have there. And I actually want a full round fillet. So, I'm going to choose this face, this face and this face over here. And that gives us a preview of what we're going to see. It's going to be a full round between all 3 of those faces. Click on OK. Alright, looking good. Now we're going to add a fillet to this corner in here, but we need to take a look at the actual radius on the outside of our sheet metal part, and we have to match that.

So let's go over and measure it. Go back to our part, let's grab the Evaluate toolbar. Grab the Measure tool, and let's spin this around and measure this radius. It says the radius here is eighth of an inch, or 0.125, and that's what we want to add that radius to in the part. Exit out of that tool, let's go back to the part and come up here to Features, Fillet. Constant radius, and let's choose a 0.125. I want it on that edge there, as well as this edge over here. And click OK, and I do want to keep that as a separate feature, so I can go back and edit this if I needed to use a different thickness in material. Let's go ahead and add one more fillet.

And 0.125 is fine and fill it all around the outside of that. Click OK and there's our tool looking pretty good. However, right now even though the tool is complete, we need to add it into a forming tool so let's go over to sheet metal, let's click on forming tool. The first question is the stopping face and that's the face down here, I want to actually push into the bottom surface. Next is faces to remove and I want to remove everything that's not actually going to be forming that gusset. So, this face, this face, this face, this one, spin it around.

Grab the top, the back, the side and the bottom. So all that will be removed. And this will fill it right there. Okay, looking good. Now insertion point. And this is very important, so pay attention to how we're going to place this. First off click on the space bar, click on normal two. And you notice this little point right here that's highlighted in blue. I want that point, which is my insertion point. To be dragged up and put right off the origin, so right on that inside edge of where we're going to be putting on this edge of the Sheet Metal bracket.

So you can see it's going to be right there at the origin, and that's how we're going to align this with the edge of the part. When you're happy with everything there, click on OK, and now we've got ourselves a form tool for an edge gusset. Let's go ahead and save that out, Save As. And I'm a call this one, 6.4 Tool 2. Because I already got one tool created and this'll give me the second one. Click on Save and then let's go ahead and add this to our Design Library. So, click on Design Library, notice I already have existing gusted in here. I want to add one more.

So come up to the plus to add to library. I select the entire tool. I'm going to call it gusted two. I'm going to add it to the ribs folder of the forming tools and go ahead and click on OK. Take a look over here in the library. You can see there's the gusset two. Looks good. Go ahead and close that part. And we're going to go ahead and push that part into this corner here. So let's remove the the gusset we have. And let's add a new one.

Spin my part around. Open up the design library. Grab that gusset, drag it out to the window. Snap it onto that lower face. He knows it showed up backwards. That's okay. Click in the rotation angle box. Type in 180. And then come over here to the positions tab. Now, we place that little orientation right at the back edge. So click on Space Bar. Click on Normal, too. And I want to turn the point tool off. And then just drag that point right up to that back edge and I could even snap to the midpoint if I wanted to.

And don't worry about this extra line here those just kind of move around with the tool, so all we're really concerned about is that orientation point when your happy with that click on OK. And there you have it. We formed that gusset right into that corner. And we built our own custom tool. Now if you're going to go and use this tool for other sheet metal thicknesses. We might go back to that gusset. Open it up, I can just go back to the gusset here. Right-click on it, click on Open, and we can adjust these radiuses in here so that they match the exterior radius on the sheet metal part we're going to be using the gusset on. When working with gussets across bends, we need to pay close attention to the material thickness and the flexibility of the material. Gussets are great features to use however, they are also easy to mess up in solid works so pay close attention to all the different features and radiuses.

There are currently no FAQs about Sheet Metal Design with SOLIDWORKS.

 
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