Automatic Extrusion from Standard Parts

[willKRURR]

Afternoon All,

I'm hoping that one of you will be able to help me with my current predicament.

A bit of background before I start.

I have been tasked by my company to streamline the Estimating, Design and Production process for Flight Cases that we produce in house.

I have successfully created the shell of the case by linking all the individual components to Length Width and Depth Parameters. Which allows me to change the overall size of the case relatively quickly.

My current sticking point is when it comes to the addition of fixings on the case (Latches, Hinges, Handles, Etc). They are all premade supplied parts which I have the individual Cad Models (Step) for. I am looking to automatically add in cuts into the extrusion/panel at the part level. Wherever one of these fixings is placed. So that further down the line I can using inventors nesting software to automatically generate DXF Machine files. I'm looking to have to do as little physical input for each part as possible as these cases can come with multiples of each fixing depending on the end user’s requirements.

These cuts also are not an exact match to the profile of the part itself. So, to the best of my knowledge copy object and then sculpt wouldn’t work.

Take one of the handles as an example. (This cut-out I have done manually.) The fixing holes are an exact match, but the main cut-out is simplified from the main profile of the handle.

If you need any more info just let me know.

Kind Regards

Will.

[SharkDesign]

Unless you're going to do a load of iLogic you can't have it cut holes just by placing items. 

You could however use ifeatures to store all your predetermined cut outs and just use the right one. 

If you always have the same hardware in it just have that driven too. 

You could also have some simple iLogic that suppresses holes that are not needed when a user selects a particular model of case. 

I assume you are using this method to drive your sizes from the top?

https://youtu.be/8qu7jwK9M6k

[mcgyvr]

Yep you are going to basically need to create all possible cuts/holes as needed and then use logic to keep or suppress them based on your options choices..

Quick example is a User Parameter (True/False) named "IncludeHoles" and Hole1 in a model.

A simple ilogic rule set to be triggered "Any User Parameter Change"

If IncludeHoles = False
	Feature.IsActive("Hole1") = False
Else
	Feature.IsActive("Hole1") = True
End If

[johnsonshiue]

Hi! On top of what James and Brian already mentioned, there isn't an automated way out-of-box. Certainly iLogic and Inventor API can help. But, it will take some time to develop the rules and the program.

One workflow may help facilitate the process. I believe you want to use Copy Object command (3D Model -> Modify -> expand the panel). This will link the premade lock geometry to the panel for positioning purpose. Then you can project the linked geometry to create holes.

Based on my understanding of your request and the model you are working on, you may want to look into Fusion 360. You can easily create the model within one design and reference geometry relatively easily.

Many thanks!