Inventor iLogic for Cabinetmaking – Placing and Configuring the Cabinets

The iCabinet test model is far along enough along to do a pretty good test of cabinetry placement and component creation. The model is a single Autodesk Inventor .ipt (part file) that is driven by 21 iLogic Rules. It has 100 solid bodies, but the amount of actual parts outputted upon component creation will depend on how each individual cabinet is configured. The final cabinets will likely average 70 parts or so each.

The test kitchen layout is a very simple corridor or galley style kitchen. I chose this style because I do not have a corner cabinet as of yet, and this is all that is really needed for the test at any rate.

This layout calls for 10 base cabinets, all of which will be created from the single iCabinet iLogic driven part. This particular design has leveler legs on the front of the cabinets and a ledger or cleat at the back on the wall as can be seen in the image to the right.

In the image below, you can see that the folder for this test contains only three items at this point…

…the Galley Kitchen assembly which is the master assembly, the Layout part that describes the floor-plan and elevations, and lastly, the iLogic driven iCabinet itself, which has been named Cab for this experiment.

Upon placing the iLogic parts, new versions of the Cab part will be created automatically with the suffix _##. I will re-size the widths of these according to the dimensions on the layout as part of the placement process. The first cabinet, located in the lower-left corner in the image below, is 16.5″ wide.

On the Assemble tab, I click the little ‘down’ arrow below the ‘Place’ command to access the ‘Place iLogic Component’ command. Withh the command active, I double click the iLogic Cab part. This brings up the iLogic part in a little window, along with another window containing all of the key iLogic parameters….

At this point I just needed to change the overall width to 16.5″ and wait for the iLogic code to execute. The amount of waiting time varies depending on what needs to happen in the configuration, how well the code is written, and likely other factors.

The image above shows the configured cabinet constrained to the layout (the dimension visibility of the layout was temporarily shut off for clarity). The image below shows all 10 cabinets in constrained in place and configured as needed.

As you can see in the image below the program the program has created new iLogic parts with the suffix I mentioned earlier. Also notice the different file sizes.

Now the parts need to be turned into individual assemblies…

..by double clicking one of the ‘smart part’ cabinets I isolated it in the assembly as shown in the image above. Then on the Layout Panel on the Manage Tab, I clicked on the Make Components tool to start the procedure that will get the actual parts created. I was then presented with the Make Components: Selection dialog shown below…

There are a couple oddities that come into play at this stage. First, you can select sketches in the browser window, but they will not be added to the selection box because they are not valid bodies or blocks. Not sure why you are even allowed to do so. What you need to do is expand the Solid Bodies folder (or the Blocks folder) , and select the bodies or blocks there or in the workspace.

This is where the second oddity comes in. Although a great deal of the solid bodies in this model are suppressed, and therefore not available to the Make Component command (a good thing), there is no visual clue as to which is which in the solid bodies folder. Just a bunch of yellow blocks. You would expect suppressed bodies to be greyed out with a line through them like features in the rest of the the Browser Bar. All bodies between the selections in the image to the right are suppressed, and cannot be selected, but there is no way of knowing this by looking.

So…… ..if you want to select items, you need to just try them to see if they select or not. If they are available, they will be selected, if not, nothing happens. It works, but is somewhat incongruous with the rest of the program. Also, if you select a body that was already selected previously, you will loose all of your selections –a real pain in the ass if you are towards the end and there are hundreds of solid bodies in the mix.

The other alternative is to select the bodies in the workspace. This may not be possible in a case where there are internal parts that you do not want to select, but a properly designed iLogic ‘Smart Part’ should have only the parts you need once configured, as is the case here.

What I did was window select the entire part as shown in the image below…

Every unsuppressed part will now be selected, and will show up in the little selection window on the Make Components dialog as shown below….

Notice the Browser Bar where you can see the gaps in the selection. The non selected parts look as though they could be selected don’t they?

Now for another stumbling block. You have two choices as to the output at this point, and neither are desirable. Although the configured iLogic part is already where it needs to be in the assembly, it cannot be transformed into its components in situ. The choices available are to create the pile of separate parts in the assembly, or create a new assembly outside of the assembly. The second option is out as it would require you to find and place the assembly a second time. Either way the assembly will need to be re-constrained to the position where the iLogic part currently sits.

So I let the program pile the parts into the current assembly as single parts. The dialogs default to this setting, so I just needed to select Next — which brought up the Make Components: Bodies dialog shown below.

This dialog allows you to fine tune things by renaming the individual parts, changing their BOM structure, changing the part template used to create the part, and changing the save location if need be. If left alone, it will give the parts the same name as the solid bodies in the part’s Solid Bodies folder –which is what I did.

Using this scheme, the program will add the suffix _1, to the next set of parts, then _2, and so-on for all remaining component creations. This is because the program detects the previous parts created, and will not make duplicate parts…which is a good thing.

Unfortunately, because the same bodies are not created for each cabinet, the suffix will not denote what cabinet the part belongs to. More control over the naming scheme beyond manually entering hundreds of names in the Make Components: Bodies dialog is a much needed feature!

Also note that you can mirror and add parameters at this point as well, but I won’t need either for this test, so I just clicked Apply.

The result is shown in the image to the right. Below the Cab-10 iLogic part, there are now a pile of new solids —– 56 to be exact. If I were to just keep making parts this way, there would have been over 500 parts floating around in the master assembly by the time all was said and done, so I nneded to create assemblies as I went.

To do so, I just selected all of the parts just created, right clicked, and chose Component > Demote. This brought up the Create In-Place Component dialog where I named the new assembly Cabinet 01…

…after clicking OK, the parts were now contained in a new sub-assembly…..but, unfortunately, it jumps to the origin of the iPart it was created from…..which in this case is in the center of the layout. The highlighted cabinet in the image below is the new assembly located at the origin.

There needs to be an option to leave the new assembly oriented in relation to the iLogic part, but I can’t think of a automatic workaround that will do so at the moment.

The remedy is fairly easy, but a pain in the butt nonetheless — just turn off the visibility of the iLogic part, then constrain the new sub assembly (Cabinet) into the opening created by the now invisible ILogic part. Not hard, but it’s extra work, and opens the door for mistakes to be introduced –especially if the Make Components part of the procedure is done by a different person from the one who placed and configured the iLogic parts.

Now the freshly made cabinet assemblies need to be broken down into sub assemblies e.g. frames, doors, drawers, etc. I will cover how to do so in the next post, and show a different naming scheme for the solid bodies that may allow the automation of same. Then it is on to the drawings, and attempting to automate that process as well.

Before I forget and delete the files, here is that same folder that contained just three parts at the beginning of this test. There are now 585…

The next post will follow later today. I will be posting a link to the iCabinet iLogic part as well, but if you would like it sooner, email me, Mark, at the address in the footer and I’ll send it to you right away.

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