To start creating a part file, we’ll click on the New button, and locate a predefined template file from the Metric folder. We’ll scroll down and select Standard (mm).ipt from the list. Once our template file has loaded, you’ll notice that we are immediately sent into Sketch Mode. In the sketch, you’ll also notice that we are automatically put on the XY plane to create our first sketch.
Accessing the Line tool on the far left hand side of the Ribbon, we’ll place our starting point anywhere we like in the Graphics Window and start to draw a 6mm vertical line.
Inventor will intuitively place geometric constraints on your geometry by snapping the line to a horizontal or vertical constraint. Once you’ve placed your point of origin for the line, you’ll notice to the left of your cursor, a field with a length, and to the right of the cursor a dynamic field for the angle of the line. You can toggle back and forth between these two fields by hitting the Tab key, and then place the required information into the field by typing it in with the keyboard. For now, we’ll direct our mouse straight up from our first point and give it a measurement of 6mm. Simply type in 6 and press Enter on your keyboard. You’ll know that the line is vertical by the constraint icon that appears temporarily beside the line you’re about to draw.
With this first line drawn, we’ll make our next line 24mm to the right by typing in the length, followed by a line 27mm going down. Make sure to use the geometric constraint guides to ensure your lines are perpendicular.
Draw another line any arbitrary number to the left of this last line, and then close the profile by clicking on the base point of our first line.
You should now see a dimension on each line that we gave an exact measurement to. Since we didn’t use exact measurements for the two last lines we created, we’ll want to make sure the second last line we drew is 10mm. To do this, we can simply add a dimensional constraint by clicking on the Dimension tool on the ribbon, select the line you would like to dimension (bottom line) and then pull the dimension off the line and centre the number to the middle of your dimension line. Now, by clicking on the number of the dimension, you activate a dialog box that allows you to enter an exact number for your dimension. For this number, we’ll type in 10mm and hit the Green checkmark. Notice the length of the line is automatically updated.
With all this complete, we can now click the Finish Sketch button at the top right of our Ribbon. With the sketch complete, Inventor will move us into an Isometric view and we can now create a feature from this sketch.
With the Sketch complete and in our Isometric view, you’ll notice that we are now in the activated Model tab, where there are many helpful tools to start our model. By choosing the Revolve command from the Create panel, you will activate a dialog box in which you define an axis of revolution as well as a profile. In this situation, because we only have this one sketch, our profile is automatically selected, however if you click on the Axis button, and hover your cursor over any line on the sketch, you’ll see it highlight. With the Axis button enabled, click on the 27mm line and notice the temporary solid that is displayed. By default, you are given a full 360 degree revolution. Once the revolve tool has been activated, there is a yellow arrow that appears that can be used to manually place the angle, or you can type an arbitrary angle into the field that currently says (Full). For our part, we’ll simply leave it as (Full) and hit the OK button in the dialog box.
Our next step is to apply a chamfer to the top edge of our nozzle part. Use the View Cube to navigate to a view where you can see the larger circular face. From the Modify panel in the Model tab Ribbon, you’ll see a Chamfer tool. Click the Chamfer tool, and then select the large circular edge as shown below. Once you’ve selected an edge to chamfer, you will be prompted to either manually execute the chamfer, or enter a precise number value for the chamfer width. By default the chamfer is set to 2mm, this is what we’ll use.
Now, in order to complete our part, we’ll need to create a hinge point at the bottom of the nozzle. To do this, we’ll want to use the same sketch as we create before, but right now, it is consumed by the Revolve feature that we first performed on it. So, in order to use this same sketch, we’ll expand the Revolve feature by clicking on the [+] sign beside the Revolve in our Model Browser, and select the Sketch. With the Sketch selected, right click and choose Share Sketch. This will allow us to use the same sketch, but it will not interfere with the feature we created with the original. Notice a new sketch is placed above the Revolve feature in our Model Browser.
Select this new Shared sketch, right click and select Edit Sketch. This will bring us back to our XY Plane, and back into Sketch mode. Again, we’ll access the Line tool, and start a line from somewhere below our bottom 10mm line, and draw it to connect to this line. We’ll draw another line from this point to the right at any length, and then another one down till you see a dotted line appear showing you that it’s in line with our first starting point. Left click to complete the line, but before you leave the command, hover the cursor back to the end point of your last line, click and hold down the left mouse button. You’ll see the yellow end point turn grey, and it will activate the arc tool. With the left mouse button still held down, bring the cursor over to the starting point of your first new line, and watch as you create a perfect semicircle.
Once you have the basic shape, apply a dimension of 6mm to the arc, 10mm to the side, and from one side to our axis of revolution in the previous sketch, place a 6mm to ensure it’s at the half way point.
With our new sketch complete with dimensions, we’ll click on the Finish Sketch button again, and to add mass to this element of our part, we’ll activate the Extrude command from the Create panel in the Model tab.
With the Extrude dialog box open, select the profile we just created from our sketch, and use the option to extrude symmetrically from both sides of our chosen profile plan. Enter a value of 12mm into the Distance field and make sure the Join option is activated and not Cut or Intersection.
We’ll repeat this step, to hollow out the centre, simply click the Extrude command again and change the Extrude option to Cut, and the enter a value of 6mm for the distance, and click OK. We should now have two prongs for our hinge and now we simply have to create a hole for the pin of the hinge.
For the last feature of our part, we’ll activate the Hole command in the Modify panel. For Placement options, in the drop down menu, choose Concentric, and for the Profile, we’ll choose the top plane of our Hinge extrusions. By choosing the curved edge of our extrusion for the Concentric reference, we’ll know that our newly created hole and the arc we used to create our extrusion shared the same centre point making the hole exactly centred. With this action, we have complete our part.
Stay tuned for our next post, when we explore the processes of taking parts and creating an assembly file to show how they interact with one another! Thanks for reading.
Travis Van Clieaf