Understand how to build the arm of a lampshade using Autodesk Inventor. This piece discusses detailed steps on how to create sketches, dimension and constrain them, and add holes to the lampshade arm.
Key Insights
- The article provides a detailed guide on creating a lampshade arm using Autodesk Inventor, starting with creating a new component then sketching the design.
- Dimensioning and constraining are essential steps in the process, ensuring the rectangles used in the arm's sketch maintain the same thickness and fixed width of 90 millimeters.
- The process also involves adding holes to the lampshade arm, which can be achieved by placing points and adding holes or by using a sketch, creating circles, and using the extrude function.
In this video, we will build the lampshade arm. If you will, please open step 3, lampshade arm.
And when your file is open, hide the data panel. We will be building our lampshade arm off to the side, rather than in place. I'll move my view over here and go to my arm assembly, right-click, new component.
I will name this lampshade arm. And let's get started. I will go create sketch and host the sketch to the bottom plane.
For this example, I will use five separate rectangles to draw my arm, and then we will dimension and constrain them. I'll move my view down to here, and let's start by drawing a rectangle. I'll just draw it any size and zoom in, D for dimension, and let's dimension this with a thickness of T. And for now, I will leave this width non-dimensioned.
I would also like to select this line and this line and go to fix, unfix. This will turn them green and will constrain this bottom line. We will be constraining and dimensioning all of our rectangles, but without fixing two of these lines, they will still be able to move around the screen.
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Let's continue with drawing our rectangles. I'll go back to rectangle, select here, here, here, and here. I'm not worried about the sizes.
I will constrain and dimension them now. First, let's go colinear, and I'll select here and here, and here and here. Let's continue with our dimensions.
I'll go D for dimension, and I will select each of these top lines and click this dimension to apply the function. Remember, this function is thickness T. Now, all of my rectangles will have the same thickness, which is our thickness user parameter. Now, I know that my lampshade will have a fixed width of 90 millimeters, so I'm going to click the inside to the inside here and type 90.
Now, I will click the outside edge here, and this will be a dimension of 70, and here, and this will be a dimension of 45. Notice that the bottom portion of my lampshade is completely dimensioned and constrained, and all of the geometry is black. However, the top geometry is still blue, meaning that I can slide it side to side.
In order to place this exactly symmetrical about the middle, I need to draw some construction geometry. I will turn on my construction, go to line, and draw from the midpoint to the midpoint. This will make a black dashed line as it is snapped to the midpoint and midpoint, and is construction geometry.
I will now go to the symmetry, and select this line, and this line, and then third, I will select my construction line here. This will place a symmetrical constraint around the center of this line. Now, as I drag, you will see both rectangles move symmetrically about the center of that line.
We know it's the center again because of the midpoint constraints. Now, if I go D for dimension, and go from this line to this line, I can type W for width, and now this distance will automatically update with my width, and will stay in the center of my lampshade arm. Everything looks fully dimensioned and constrained, so I'll hit stop sketch, return to my home view, and let's use the extrude command.
I'll go extrude, select this inner body, and drag up W, enter. Let's turn our sketch back on, and go extrude one more time. I'll select the remaining four profiles, drag up W, and before I hit ENTER, I need to make sure to change my operation to new body.
Saying that I have W as my distance, I'll hit OK, and turn off my sketch. Finally, we need to add the holes in our lampshade arm. We can do this by placing points, and adding holes, or by using a sketch, and creating circles, and using extrude.
I'll create a sketch, select this face, and go C for circle. I'll draw one circle here, and one here. In this geometry, I don't really have good circles to get my exact diameter from, so I'll go D for dimension, and type in D for diameter.
Here, I'll click this function to update that dimension. I can now go horizontal vertical, select my two circles to snap them horizontal, and select this circle, and hold shift to grab the midpoint here to snap them exactly in the middle of my part. I'll go D for dimension one more time, and dimension the distances for my circles.
This will be 22.5, and this will be 15. Again, this is a static dimension, and should not be influenced by my user parameters. I'll hit stop sketch, and let's go extrude to finish the model.
I'll select these two profiles, drag so that I see the red direction, and change my distance to all. This will cut through everything in my model, and if you notice, I drew my geometry past my lampshade body, so that it's not cutting through the base. If yours was drawn over here, and is cutting through the base, check your objects to cut, and make sure that only lampshade bodies are being cut with this command.
I'll hit OK, go to my home view, and activate my main component. I can now group these objects in my timeline, and save my file. In the next video, we will use joints and as-built joints to assemble our model.
I will see you in the next video.
