Manage sheet metal designs

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Manage sheet metal designs.

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After completing this video, you'll be able to

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demonstrate the ability to create a sheet metal part using sheet metal tools,

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create or modify a sheet metal part using critical tools,

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and utilize sheet metal defaults window to get desired results.

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To get started, we want to open the supplied dataset, sheet_metal_creation.IPT.

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We're going to be taking a look at modifying some of the features, creating our own features, and also talking about the sheet metal defaults.

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When you're working with a sheet metal part, you have the option to modify your sheet metal defaults.

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The sheet metal defaults, or rules that apply to your sheet metal designs,

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will contain information about things like the part thickness, as well as rules for how the bends are created,

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what the K factor is to determine the amount of material for your flattened pattern,

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as well as other considerations for what happens in corners and with certain types of bends.

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We can modify these values by using the pencil icon to the right of our sheet metal rule

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or select additional rules that are already in the design.

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Let's go ahead and select the Default and go to the pencil icon to make our modifications.

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Once we select the pencil icon, the Styles and Standard Editor library will open.

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Notice that this is set to Read/Write currently.

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You may not see Read/Write permissions on some of your Styles and Standards editor.

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That will depend on your permissions, the way your project is set up, and also what you're doing at the time.

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The sheet metal rules generally are able to be overwritten,

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but you may want to double check your project settings if you only see a read access option inside your library.

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We're going to be taking a quick look at some of the values inside of our Styles and Standard Editor,

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so there's no need to make any modifications first.

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On the first tab we have Sheet.

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This is going to list our material, which we can select a specific material if needed.

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For example, if we're going to be working with an aluminum material,

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we can navigate to aluminum inside of this list.

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Keep in mind that certain types of aluminum are better for bending than others.

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But for the purposes of what we're doing here, just note that we do have the available options to change our material.

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We can also modify our thickness value by manually entering a thickness or measuring it on the design.

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In the lower section here we've got our Flat Pattern Bend Angle.

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This is basically telling us whether or not we're reporting the bend angle from the inside of our part or from the outside of our part.

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We also have some options for how formed or punched features will display on a flat pattern.

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Notice the Unfold Rule is set to K factor by default.

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We also have bend compensation, and again, we have a pencil icon that allows us to modify these values.

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We're going to move over to the Bend section.

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In the Bend section, we can see that the default Bend Radius is based on our thickness value,

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but we can override this as well by manually entering a value.

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The Relief Shape by default is straight, but we have other options here as well.

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For the most part, these defaults are going to stay throughout all your designs,

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but if you have a specific reason, you may find the need to change these.

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Next, let's take a look at our Corner.

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When we take a look at our corner options, we can see what's going to happen when we have two or three bends intersecting.

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For example, Trim to Bend shows our inside and outside bend lines exactly lining up with the bend relief shape.

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If we change this instead to a Square relief type, notice that the image shows the square is larger than those bend lines.

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We can also select other types such as Round or Tear, and it really is going to depend on your specific instances.

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We're going to leave this one as Trim to Bend by default.

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If you want to create a new style, it's always best to start with one of the default styles, either the imperial or the metric one,

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and then simply modify the values that are needed from there.

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Because we don't need to save any modifications, so, I'm going to select Cancel instead of Save and Close.

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And select Cancel here as well.

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Now that we understand a bit about the sheet metal defaults,

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let's go ahead and talk about modifying our sheet metal design as well as creating some of our own features.

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In this design, we've got several flanges, we've got a sketch called Cut 2, and another feature called Cut Across Bend.

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Let's begin by modifying this Cut Across Bend by right-clicking and selecting Edit Feature.

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Inside of our Cut Across Bend dialog, we have a couple of options next to the profile.

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We've got one option for Cut Normal and another option for Cut Across Bend.

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If we select Cut Across Bend, notice that our sketch is now wrapped around the outside of our part,

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creating the cut based on the overall length of that design.

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We're going to say OK, then we're going to go into our sketch, right-click, and we're going to change our visibility.

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Then we're going to modify this 1.75 inch dimension.

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If I make this 2 inches and we rebuild our document, you can see that it's increasing the overall distance of that slot.

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If we change it instead to 1.5 inches and once again we rebuild our document,

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you can see that it's reducing the overall height.

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Using this cut across bend is a great way for us to design cuts that go around a corner of a bend,

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and this is a simple way for us to develop it inside of a single sketch.

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There are other ways that we can create cuts that go across bends, however.

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In this other case for our sketch Cut 2, we want to begin by unfolding and refolding our design before and after our cut.

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So, we're going to start by selecting Unfold.

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We can select a stationary reference, which is this bottom face, and then we can pick which bends we want to flatten.

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We're going to say OK, and then we can use the Cut tool with our sketch.

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This is going to cut based on the thickness of our sheet metal part, noting that it's on the option here for Cut Across Bend by default.

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But in this case, our part is flat, so it's not going to matter.

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Then after we're done, we can select Refold, select our stationary reference, and once again collect our bends.

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Using this Unfold and Refold option to create cuts across bends is extremely handy,

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especially when your designs are going to be more complex than a simple jog like we have in this part.

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From here, let's go ahead and take a look at Cut 2.

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Right-click and change its visibility since we no longer need to see it.

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One more handy thing to understand about our sheet metal parts is the ability to toggle and change the way our flanges are created.

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Let's modify Flange 4 by once again right-clicking and selecting Edit Feature.

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In the very top section, we've got Flange edge Sets.

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Keep in mind that if you're using an older version of Inventor, 2023 or 2024, the UI and these dialogs have changed slightly in 2025,

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so you may not see exactly the same options.

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But in the edge selection here, we can see that we're going to the complete distance for our edge,

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but we also have some options to change whether or not it's using a specific width value,

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whether or not we are going to toggle it based on selected faces, or if we're going to have it offset from the outside edges of its selection.

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These are great options that allow us to configure our sheet metal flanges directly in a single operation without having to flatten them,

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make cuts, and then refold them later on.

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Let's go ahead and select OK, noting that all the rest of the features are going to update properly.

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These are just a handful of the tools inside of the sheet metal tool set.

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Make sure that you do play around with each of these tools, understand its options before you move on to taking the certification.