In the last installment of this Cabinet Configurator Tutorial, we left off with the Plan sketch nearly complete –but the side panels geometry was left only partially constrained due to the length of the post. As with the Shaker Table blogtorial, we need to create a setback in the sketch that is driven by iLogic, which will be driven to zero at some configurations. Doing so will almost always result in a portion of your model flipping inside-out when driven back to a non-zero configuration. So what we will do to stop this from happening is create an outrigger. Please use the outrigger link if you would like more info. Otherwise, let’s get to it…
Firstly, create three new parameters (shown in the image above) named Case_Side_Setback, Case_Side_Offset_Right and Case_Side_Offset_Left. The Case_Side_Setback value will be a shop standard value describing how far unfinished sides are inset from the end of the face frame. Give this first parameter a value of 1/4″, then set the other two to equal it (see the bottom three parameters in the image above). These second two parameters will be controlled via iLogic shortly for testing –hopefully in today’s installmentJ Now create a Horizontal (looking down on the Plan sketch in the TOP view) line.
Then, add a plain-ole dimension of 1″ to the new line. Now dimension between the line that represents the side of the cabinet and the endpoint of the outrigger (the line you just made), and use the formula Case_Side_Offset_Right + d-whatever. To get the second part of the equation, just click on the outrigger’s dimension and it will appear wherever you cursor was in the Edit Dimension dialog…
We are doing this because you may have a different dimension number than the d45 shown. Now change the outrigger line into Construction Geometry, then repeat the outrigger creation steps on the other side…
Smashing! We are 100% super fully constrained and pretty damned bulletproof. Now for some new parameters and then some iLogic. Finish the sketch and save, then, if the Parameter Panel is not visible, right click on the Ribbon and choose Parameters from the Show Panels fly-out. I use the Parameters editor so often that I have it added to most of the Tabs. Fire up the parameter editor and create two new Text Parameters — Case_Side_Type_Right and a left version of the same. Make the value of each Unfinished…
Now right click anywhere in the Case_Side_Type_Right row, and select Make Multi-Value. The Value List dialog will appear, where you want to type Finished into the top Add New Items section…
Click Add then OK to complete the operation, then do the same thing for the left Case_Side_Type_Left parameter.
You now have two Multi Value Parameters that do absolutely nothing. Lets remedy that with some iLogic.
Switch over to the Manage Tab, and click the iLogic Browser icon on the iLogic Panel. I generally dock it on the right as I have extra wide monitors, but you can put it wherever you damn well please –unless your boss says otherwise J With the Rues Tab active, right click in the empty iLogic Browser and select Add Rule (nothing else to select), and name the new rule Main. Click the User Parameters text in the Model Tab of the Edit Rule dialog –This populates the Parameters Tab just to the right. Type If, then add a space in the code window (lower right), then scroll down to the bottom of the Parameters list you just populated, and double click the Case_Side_Type_Right text in the Parameters list. The parameter will appear in the code window…
…the blue syntax highlighting means the text equals a valid Parameter. We now add an equals sign, then the Unfinished value within quotes to denote that it is a text string. Finish off the line with the Then statement. The next line must tell the program what to do if the above statement is true. At some point, all kinds of things need to happen, but for now, we just need to set the angle on the end of the face frame and set the amount of setback for the side panel. We need to do this for both sides…
I’ll be making a video for the next installment, in which I will explain the why’s and what-for’s of the above iLogic Code, and show how to make a quick iLogic Form for testing same. Then, I think we may go on to start creating the face frame options.
Later.
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I am very new to the interface and am experiencing a rookie problem that I presume takes a long time to fix. In 2 cases, both for the iDoor and your ERP Cabinet tutorials, I have managed to nearly finish all steps without creating a single part at the start of the tutorial as you had directed. I am obviously realizing now the extent of that problem as inventor is prohibiting me from extruding solids from the carefully followed sketches created. I am very frustrated with this, as I have done most of the work but without receiving the satisfaction of making a 3D form. Although I have not found a solution online, I am hoping there is an easy fix where I can import a sketch into a new part so that I can remedy this issue. Is there such a trick?
Hi Dylan,
This is kind of a strange one. You must have a part to create a sketch, so there is a part somewhere. Is there any way you can email or place online a screenshot of your entire interface that contains a sketch you speak of? Windows 7 has the snipping tool for doing this under Accessories. Once you do that, we should be able to nail down the issue. I’ll likely move this to the forum so that others can see the image.
Mark