Sheet Metal Design with SOLIDWORKS
Illustration by Richard Downs

Adding cuts in context


From:

Sheet Metal Design with SOLIDWORKS

with Gabriel Corbett

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Video: Adding cuts in context

When dealing with complex sheet metal assemblies with many fasteners and connectors. Creating cuts in sheet metal can be extremely complicated. If we add these cuts as in-context features, we can reference the other components and make things much easier. Let's take a look at this assembly here. I've got a circuit board here, and I've got a sheet metal enclosure that we want to cut the holes for the connector through. Now I can measure and try to align these things and get the cutouts in the correct location, but that be allot of work and be extremely complicated. Instead we can edit this sheet metal bracket in context and use those as a reference.
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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

Adding cuts in context

When dealing with complex sheet metal assemblies with many fasteners and connectors. Creating cuts in sheet metal can be extremely complicated. If we add these cuts as in-context features, we can reference the other components and make things much easier. Let's take a look at this assembly here. I've got a circuit board here, and I've got a sheet metal enclosure that we want to cut the holes for the connector through. Now I can measure and try to align these things and get the cutouts in the correct location, but that be allot of work and be extremely complicated. Instead we can edit this sheet metal bracket in context and use those as a reference.

To do so, let's go ahead and click on this part here and click on Edit Part. That will edit the part in context to the assembly, and you can see here I've got all the other components grayed out now and I'm working just on this component. You can tell you're in this mode by, this is now highlighted in blue. And I can go down here and see all the features that are making up that component. Let's click on that front face, click on Sketch. And click on Normal To real quick. Now you notice, I can see this one component here. But I can't see any of those other connectors behind. So what I'd like to do is change my display from Shaded With Edges down here to Wire Frame.

That way, I can see through and see all the components that we have in our design. Next, I want to use the Corner Rectangle command and I'm going to come up here and I'm going to draw a rectangle around this component here. And I'm going to snap to the top of that circuit board down here. Now I can add a few dimensions. From the top of the connector to the top of the hole, maybe 20 thousandths of space and I'll do the same thing a couple more times. And the cool thing about adding in dimensions and relationships in context is if we go back to that circuit board. And we move this component around later, those will automatically follow wherever this component goes to.

And that was a pretty simple thing. We just added a box. But how about over here? We've got a component here that's got some rounded corners, some angles. That'll be a little bit harder to draw our ourselves. So we can use the Convert Entities command. Let's go ahead and click on Convert Entities. And we can choose these lines that go around the outside of the part to bring over and convert. Okay? When they're all selected, go ahead and click on OK. And that brings those into our current sketch. And then I can use those as an offset. I'm going to offset by that same 20 thousandths.

And go ahead and click on Make Base Construction. That way, the existing entities here will just be for construction lines. And we'll only be using this one new line that we're creating. Add the 20 thousandths, click OK. And there's our new line. And then over here, similar kind of thing. We don't have a perfect profile to follow along out here. But we can use a little bit of exterior referencing as well. I'll create a rectangle. Snap around the outside other part. We'll add a few dimensions, may be from this edge here to this one here. 20 thousandths, top and bottom.

And over here as well. Now I might want to make it look angled cut on this side here. So I can add an in context cut, across there, we can make a relationship between this line. Hold down Ctrl on that line, and make those parallel, for one thing. And we can add a space between the two. Again, 20 thousandths. And this time I'm going to use the Trim tool and just trim out that corner. The only thing that happened here is this blue line at the bottom.

Because I cut off that corner, it's now not snapped there, no problem. I can move it up, bring it back down, snap it on that corner, and there's our cut. Now we can add fill its in here if we want to or make any other changes to our cuts but so far, looks pretty good. Let's go back up to Features, let's do an extruded cut. Because we're working in sheet metal, we can use this Link To Thickness. Click on Link To Thickness and it's going to go ahead and cut through that first level of sheet metal. Click OK and let's switch back to Shaded With Edges.

You can see I've got a couple of cuts there, and come back to my assembly. And they're there. Cuts perfectly around the connectors and things are looking good. Let's go back and see if we can make the cutouts follow the connectors if I move one of the connectors on the circuit board. Let's click on this assembly here. Let's open the assembly and maybe this connector here. Let's look for its mates. You can see there's a distance made from the edge. And let's go ahead and move that, instead of 2.5, let's change it to 2.25.

Click on OK. That moves over. Let's go back to our assembly. Rebuild. And you can see it just follows that along. So I can move any of those components and it makes it very robust design. They have all your cut outs, follow your connectors. Especially when you're working with circuit boards or any other type of components that are going to be rapidly changing or changing often. It will really save your lot of time in the long run.

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