Is it possible to add a feature (extrusion) to multiple files at once using a excel to define the parts.
Hi @J.VandeMerckt. It is certainly possible to make a list of files in an Excel file, and have an iLogic rule look at that list of files, to know which files to process. The hardest part though, would be the rest of the task. Specifying a plane, starting a sketch on that plane, sketching the needed geometry in the correct location and orientation, in a way that is recognized as a closed profile that can be used for an extrusion feature. Then creating the extrusion feature itself, based on that sketch, with the correct dimensions & settings. There are several specifications, numerical values, and settings involved in that task, so I'm not sure how you would lay all of that out in an Excel file. There may be a way to just copy certain aspects of the task from a previous model to the next model, before closing the last one. I know you can copy sketch geometry that way, but I don't think you can copy an entire extrude feature that way directly. Have you considered making the feature an iFeature, that way you can quickly, and easily place that same feature into many other models?
Wesley Crihfield
(Not an Autodesk Employee)
Unfortunately, I do not think there is a built-in Tutorial guide for creating one of them, but you may find a video on YouTube about them. They can be quite useful though, so it is definitely something worth looking into. They can range from very simple to complex, so creating them can also be either somewhat simple or pretty complicated. You start with new feature that you create normally. But it is definitely important to keep in mind that you are creating the feature for an iFeature, because some stuff may need to be done a bit differently than usual. For instance, you will want the sketch plane, constraints, dimensions, and such to be as independent and modular as possible. You will also want to rename every Parameter that gets created for each dimension you place in it, so that you know which parameters are for which aspects of the sketch. If you need to base your sketch off of some projected model edges, keep those types of things as minimal as possible, and remember precisely which edge it is being offset from, because you will need to know that later. Then when you create the extrude feature, there will be parameters automatically created at that time too, for things like extrude extend, angle, and such. Find and rename those parameters too, so you know which ones are which.
Then on the Manage tab, go to the Author panel, and choose the tool named Extract iFeature. This is where you can choose the feature, its sketch, the parameters involved, the reference model edges involved, and provide prompt type descriptions and names to those items, and set the order in which those things will be asked for when you go to place the iFeature in another model. Make sure you are as clear as possible in this extraction process, so you will know what you intended a year from now. Make sure you save it in one of the designated locations, such as the 'Catalog' folder under your "C:\Users\Public\Documents\Autodesk\Inventor <VersionYear>\Catalog\", because that is where it looks for iFeature and sheet metal punch tools by default.
Once that process is done, and the iFeature file is saved out, you can open another model file where you would like to place that iFeature, and on the 3D Model tab, you may have a panel showing namd Insert (if not, you may have to show that panel), and it may have a drop-down list. Choose Insert iFeature, then navigate to where you saved that iFeature file. Then follow the prompts where it wants you to select those same edges on that other part for what plane to put the sketch on, what edge(s) to offset from, what parameter values to use (some may not need to be changed, and are retained), etc.
Wesley Crihfield
(Not an Autodesk Employee)
OK. I'm not sure if iParts can contain iFeatures, or how well they may 'play together' if they can be used together, because it has been years since I used iParts that much. I know that both iParts/iAssemblies and the new ModelStates are still both present in the newer versions of Inventor, and that there is a balancing act for which direction is best, usually based on quantity of variations. If there are fewer variations, then usually ModelStates will be better the better option, but when the number of variations gets to a certain point, the iPart/iAssembly route starts looking better. And I'm not sure I would completely take the iLogic thing off the table, either. It may be challenging, but only you can determine / decide if it would be worth the while to invest in.
Wesley Crihfield
(Not an Autodesk Employee)
If you have more than a thousand variations of the same thing, then iParts definitely sounds like the way to go to me. (Feel free to get more opinions though.) You can edit all values in an Excel spreadsheet that way. However, from what I recall, if you have already generated dummy model files for most, if not all variations in the table, I do not remember if those dummy model files will automatically update when you change the table values in the main iPart factory file. You may have to re-generate the model files from the iPart factory file, based on the changed values in the table. I am not sure if that model file regeneration process may break any assembly constraints where those pre-existing dummy model files may currently be used in existing assemblies or not. Maybe something to test on a small scale.
Wesley Crihfield
(Not an Autodesk Employee)
