Inventor Tutorial – Layout Part Creation – Side Elevation – 1

In this, the first Inventor Tutorial in the Automated Cabinetry Configurator Blogtorial Series, we will begin with the creation of the Layout Part’s elevation sketch –but before we do that, I should briefly explain how our model will relate to the 3D space we will be modeling in.

Inventor uses a Right Handed Cartesian coordinate system, whereby your base plane is XY with the Y axis pointing up towards the top of your monitor, the X axis pointing to the right, and the Z axis pointing out of the computer monitor towards you. The model would come out the same no matter which coordinate system is used, but we need to stay on the same page if you want to end up with a working model at the end of this blogtorial.

In the video below I will go through the steps of starting the first sketch in the Layout Part. This part will control the size and location of everything in this model…

 

I have designated the drawers and doors to be purchased components, but the same info can be used to create the components in-house. In reality, the entire unit can be configured to be purchased if you have decent vendors for the them. When the blogtorial is over, you should be able to adapt the model to whatever your needs are –or even steer the blogtorial itself in that direction. I only have a rough idea where this will wind up, and will use comments to steer the series where possible.

So let’s get to it. If you followed along with the video, you should have a sketch on the YZ Plane. Make sure the View Cube says RIGHT, and that the word in not upside-down. The UCS indicator should have the green Y arrow pointing up, the blue Z arrow pointing left, and the red X arrow pointing at you. Before I forget (again), I named the part Automated Cabinet Design. If you named yours something else, please rename it before we get too far down the road…

 

 

The part is split down the middle by the YZ Plane that we are now sketching on for a reason, so that we can mirror things from one side to the other in an elegant fashion if we so choose. The other two planes are not that cut-and-dried. For this model, there is no reason to place the XY (default FRONT on the View Cube) plane down the center of the part as there is nothing (I think) that is mirrored from front to back. It makes far more sense to locate this plane on the outer face of the face frame. The bottom plane (XZ) will go…….at the bottom –but would go in the center if there was a lot of mirroring to do. Planes need to go where they make the most sense for the part being created.

The cross we see in the canvas is the edges of the front and bottom planes. The center is the Center Point. If you hover your cursor over the XZ and XY planes in the Browser, you can see what is what…

 

 

If you have figured out that the model must be up and to the right of the centerpoint, you are correct!

To define the overall height and depth, we will simply draw a Two Point Rectangle (Draw Panel) starting on the Center Point (wait until you see the green dot, then click), and going up to the right. Size is not important, just click somewhere up to the right…

 

 

 Notice in the status bar on the lower right. I tells us that we need two dimensions to fully constrain the sketch. All sketches should be fully constrained, and we will do so here. I have run across acceptations to the rule, but they are few and far between. I don’t have time to go into the why’s and what-for’s at the moment, so for now, just trust me and ALWAYS fully constrain your sketches. To do this, we will create two parameters, and use them to define the two dimensions. Click the Parameters Tool on the Parameters Tab to open the Parameter Editor. Click the Add Numeric button on the lower left, then type in Overall_Height in the box in the Parameter Name column. Make absolutely sure the spelling is correct, and that the underscore is present between the words. There can be no spaces or special characters in parameter names, and an incorrect spelling is likely to cause some iLogic Code to fail down the road. In the Equation column, give it a height of 36. There is no need to add the ‘in’ because the we used an inch template. Create the depth parameter the same manner as seen below…

 

 

 Now we can add dimensions to the sketch to fully constrain it. Click on the Dimension tool (Constrain Panel on the Sketch Tab), then click the top and bottom end points of the right vertical line…

 

 

Do not click the line itself as we will likely be dicing and slicing this line to bits later on, and you will need to re-dimension every time if you choose the line. After selecting the endpoints, the Edit Dimension dialog will pop up. Click the itty bitty arrow head to the right of the text box to get to the list it hides. On that list, choose List Parameters. The Parameter list box will pop up –all you need to do is click the right one, which will add the parameter to the Edit Dimension text field, then click the green check mark to accept the value.

If you have used older versions of Inventor, you will notice that what happens next is a new feature for Inventor 2013. The first dimension added to a sketch now scales the entire sketch to the dimension instead of blowing the crap out of it. I’ll cover this in-depth in one of the new features for 2013 posts I’ll be doing, but for now I’ll just say it’s about time. If you look down in the status bar, it should, somewhat goofily read “1 dimensions needed”. We will add that 1 dimensions now. Add the Overall_Depth parameter to a dimension on the bottom line. I don’t think this line will be chopped up, so it should be OK. Just grab the Dimension tool, click the bottom line, drag down, and release. Add the parameter in the same manner as the other, and you should have this…

 

 

 

 

 

If you look in the lower right, you will see that the sketch is now fully constrained………. and, new in Inventor 2013, we now have a visual indicator as to whether a sketch is fully constrained in the browser as well! See the little orange push-pin in the sketch icon? (left of the Side Elevation text in the image to the right)

This will allow you to see at a glance if your, or your sloppy modeling coworker’s, sketches are all fully constrained. Great for both conscientious modelers and tattle tails alike!

 

 

That’s all for this installment of the Inventor Tutorial for Automated Cabinet Design. Make sure you save and close your sketch. With the preliminary stuff out of the way, we should be able to plow right into some heavy sketch action in the next installment. See you then.

Later.

 

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