How to dimension the apex of bend in drawing file
Step 1. Start a new sketch on the Right side (YZ Plane).
Sketch the three lines as shown with the Origin in upper right corner.
You can dimension the angle as 45° or as 135° as desired.
Add a sketch Point at the midpoint of the 3 inch line as shown below..
Edit your Sheet Metal Defaults...
Click on the pencil glyph
Set your Thickness parameter.
Select the Contoured Flange tool and set as shown...
Attach your progress here for next set of steps.
@julietang wrote:
... I do need to practice more using the contour roll feature.
Not the Contour Roll feature; the Contour Flange feature. Contour Flange is very similar to Extrude, while Contour Roll is more like Revolve.
Sam B
Inventor Pro 2024.1.1 | Windows 10 Home 22H2
Always use Symmetry when possible and practical.
This especially pays dividends when getting to Assembly.
I am going to demonstrate an alternate technique where symmetry is valuable.
Edit: There might be some cases where manufacturing doesn't want you to use symmetry as they don't know how to use their software and could benefit from training.
Right click or Alt c and select Create Drawing View...
Select your drawing template or a blank template.
Select the right side of the View Cube...
Right click select OK.
Right click on the view in the browser and select Retrieve Model Annotations.
You can drag these to aesthetically pleasing positions and drag the connection points of extension lines to new locations if needed.
There is an Application Option to retrieve dimensions automatically, but unless all of your parts are relatively simple you probably do not want this active.
Right click on the 3 inch dimension and select Edit Model Dimension...
Change the 3 inch to 4 inch and click the green checkmark.
You just edited the part from the drawing.
I just wanted to demonstrate that you can edit these retrieved model dimensions.
Undo that edit to go back to the 3 inch dimension.
Edit: Double click on these images above to enlarge if they are too small to see on your screen.
Next we will experiment with different ways of placing the holes...
Right click on Sketch1 in the browser and turn on Visibility.
Start a New Sketch on the inclined face shown above.
Project Geometry the sketch point from Sketch1 into Sketch2.
Turn off the visibility of Sketch1.
Sketch the two circles as shown.
Sketch the vertical construction line as shown.
Add a sketch point where shown (not technically needed - but let's add it anyway).
