Annotate drawings

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Annotate drawings.

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After completing this video, you'll be able to edit a geometric tolerance in a detailed drawing,

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place and use symbols such as feature control frames and surface,

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and manage BOM in an assembly.

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Inside of Inventor, we want to begin by opening three supplied datasets

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Engine Con Rod.IPT, which is in the assembly subfolder under the Engine Mark 2 assembly

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and the engine mark two assembly itself in the same subfolder.

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We also want to open up our Weldment assembly in the assembly subfolder under the Weldment subfolder.

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If you didn't save your weldment assembly from our weldment video,

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we want to make sure that we begin by first adding a weld.

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We're going to select fillet and add a fillet weld between the cylinder with the second selection being the top face.

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Make sure the fillet size is set to .1 and make sure that we're creating a weld symbol.

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We're going to set this at .1 X .1.

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Make sure that we are using the fillet weld symbol,

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and we're going to set the Contour as Convex.

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Also note that we have some additional options in here that we're going to leave empty for now.

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We're going to select Apply and then Cancel to close the dialog.

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We'll return and make sure that we save the weldment assembly.

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Back in the Engine Con Rod, we're going to begin by creating a new detailed drawing.

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We're going to use the standard .IDW using the empty template and select create.

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Once we have an empty template, we'll start with a base view.

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We use all the default settings and select OK.

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We'll pull the base view into the middle of the screen,

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and then we'll create a projected view off to the right hand side, right click and create.

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Often times when we're creating detailed drawings,

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we need to add specific symbols, notes, and dimensions that are required for manufacture.

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For example, adding a center mark to the center of these holes will not only help identify them as true holes,

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but also give us something to reference when we're adding dimensions.

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When we add dimensions, generally there's going to be a global tolerance applied to the detailed drawing.

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Usually this is a note that's seen in the title block area.

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However, certain geometry often requires a different set of tolerance.

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We can do this by navigating to the Precision Intolerance tab.

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We can even change our primary units and primary tolerance values, and then we can modify the tolerance method.

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In this case, let's use a symmetric value of ±.001.

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±.001 means that as we look at this dimension, we have .935 plus or minus that .001 value.

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This means the overall distance between the two holes selected can be .934 to .936.

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Having a specific tolerance value to a single dimension

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is a great way to ensure that those dimensions are going to be measured accurately

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and make sure that they fall within their manufacturing tolerances.

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If we're modifying dimensions on a detailed drawing, we also have the option to dictate them as inspection dimensions.

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Now, the inspection dimensions are going to vary based on the manufacturing methods in the industry,

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but calling out a specific dimension as an inspection dimension

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will put a specific bubble around it inside of our detailed drawing

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that allows us to identify that this dimension is critical and needs to be validated after manufacture.

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Let's talk a bit more about symbols.

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Symbols are added to detailed drawings for various reasons.

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Datums, for example, are referencing specific areas of a geometry on a detailed drawing.

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In this case, we can add a datum to this front face on our con rod.

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We're going to select OK to add a datum A.

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Let's go ahead and zoom into this area.

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Once we have the datum A, we might add a feature control frame.

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Feature control frames will reference the datum and apply specific symbols that are required for the manufacturer of this part.

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For example, we select continue to create this datum.

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We may want to have a tolerance of ±.001 in reference to datum A, and we're going to set the symbol as parallelism.

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This means that the back face of the connecting rod needs to maintain a parallel relationship with the front face of the connecting rod

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within the tolerance specified.

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Using these datums and feature control frames are a great way to call out specific manufacturing requirements for your parts.

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Let's go ahead and navigate to our weldment assembly.

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As mentioned in our weldment video, we can add weldment symbols to fillet welds inside of our weldment assembly.

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Often times weldment symbols will be added when they're created at the detailed drawing level,

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but we do have the ability to do either them in the assembly or at the detailed drawing level.

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Let's go ahead and create a basic detailed drawing using again the blank template,

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but this time we're going to create a base view for our welded part.

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We use the default view and then create a projected view off to the right and up in the isometric direction.

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We can see that these are too large for our drawing, so we'll double click on the original one and change our scale to 4:1.

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This will give us a better size reference on the detailed drawing and we'll go ahead and reduce the isometric view as well.

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When we're taking a look at these views on a detailed drawing, note, by default, the weldment symbol call out does not appear.

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If we want to manually add a weldment symbol, we can do this by going to our symbols area and use the welding option.

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The weldment symbol can attach to a weld.

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We can right click to create it and then we can fill out the weld properties.

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For example, if we want .1 of a fillet weld with the specific contour, we can add this symbol to our detailed drawing.

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However, there's a better way for us to do this.

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If we take this view for example, and go to our model tab,

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we have the option to bring in our model welding symbols and even weld annotations.

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When we do this, it'll add the welding symbol on the screen, letting us know that this is a weld and not just a fillet or a chamfer.

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It also allows us to bring in the welding symbol that was created inside of the welding assembly.

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The one downside or thing that we need to consider when we're adding welding symbols at the assembly level

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is that we can't right click and edit the symbol here.

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Symbols added at the drawing level do have the Edit Weld Symbol option.

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It's just simply important to consider the implications of whether or not a weld symbol is added to the assembly

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or the detailed drawing level.

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There's one more topic that we want to talk about when we think about using detailed drawings,

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and that's going to be a bill of materials, or a BOM.

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Inside of our engine assembly, in the Manage section on our Assemble tab, we have Bill of Materials.

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The bill of materials on the Assemble tab have model data and structured.

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When we look at this information, we have the ability to configure the way that the BOM is going to be displayed.

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But there are some key aspects that we need to understand when we're looking at the BOM in our assembly view,

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the first of which is going to be the BOM structure.

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You'll note that in this case we've got normal for our BOM structure,

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but in some instances we've got Phantom.

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When we have sub assemblies like this clutch bearing, that item does not need to have a place on our bill of materials,

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but if we expand it, each of the items inside that sub assembly are listed as normal, or in some cases we have items listed as purchased.

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There are many different types of BOM structures that we can use inside of Inventor.

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Things like References, Phantoms, versus Inseparable.

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It's important that you review the different types of BOM structures that are available so you understand what each one does.

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For example, we might have components like this phantom reference clutch bearing that don't need to appear on a BOM.

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This is because we have subcomponents or subassembly components that are included on that BOM already.

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In some instances, we might have empty or virtual components added to an assembly that do need to appear on a bill of materials.

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This may be things like hardware or instruction manuals that don't necessarily need a 3D model,

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but you may want to include extra hardware or the assembly manual in a bill of materials on a detailed drawing.

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You can add those virtual components

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and you can set them up on your bill of materials so that they do have a place in the BOM structure.

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Note that when we go to our structure tab, there are a couple of extra options.

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At the very top, we can see various configurations for members in this assembly.

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For example, there are multiple options for the rear exhaust or potentially side exhaust variations of this engine.

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We also see 2, 3, and 4 shoe variations.

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These 2, 3, and 4 shoe variations are based on the clutch set up inside of this engine.

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We can also use the All Members option which will show us individual columns and rows for all of the different instances of those parts.

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It is important to note that when we're talking about a structured bill of materials,

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if there are variations between things like the descriptions or part numbers with those various configured parts,

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you may see an asterisk in a column and it says Varies.

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When we have these options, we may need to go into our merge row settings

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and determine how we want to merge rows if there are potential conflicts.

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When we have potential conflicts, it's important to identify if those are intended or if there is a potential problem with your assembly.

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Make sure that you do play around and spend some time working with the bill of materials in the assembly

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and make sure that you do understand some of those options,

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such as things like reference, phantom and inseparable items in the BOM structure.