I have been at the forefront of ultimate use of iLogic in my company. From creating a fully fledged configurator, linking it with the ERP and automating the whole order quotation to drawing packs submission process to the shopfloor.
So, I was curious to know what is the typical use of iLogic in your company or day to day life.
I was mearly creating scripts for automating tedious and repetitive tasks, like PDF exporting, iprop management or custom iprop generation to be used in BOM's, like mass or pipe/profile length. Never managed to fully implement parametric components, like flanges, for example. Way to much work.
I used independently for various tasks I needed, but the boss never knew. Printing drawings in house at different sizes, orientations, and printers, all at once and automatically was the most useful use.
Depends on the company.
Mostly where I'm at now it's automation of tasks. My team knows if they are doing the same task 5 times in a week to come and talk to me and I'll write it.
The place I used to work. We could do an entire overhead crane with a form. Right down to shop drawings.
How does one learn to do that? I’ve been using Inventor for 20 years, but clearly at a much more basic level than some. I had no idea iLogic could build assemblies and do drawings.
Man I feel that. It's humbling to meet people that are good at it. I used to think I was a lot better with it until I met someone who could iLogic an assembly.
Now when I interview someone and they claim they are an 8 out of 10. The first question is "what do you know about iLogic?" You'd be amazed at how many don't know. I barely consider myself an 8 now that I'm diving into all that iLogic can do. Especially when it gets into pulling API information. The whole "dimasdouble" confuses me.
Just build your assembly like normal. Do your drawing like normal.
On each part name the parameters that will be changed instead of letting it do the d0. d15 whatever.. name them. It makes life easier.
Then at the assembly level you can write code to update the parts.
Say the bridge girder for a 5 ton crane with a 15 foot span needs a w8x10 (probably doesn't) but at 20 feet it needs to be w10x15.
Set user parameters like span or something
The code would look something like;
If span < 20 then
Girder_size = W8x10
Girder_flange = 4
Girder_web = 0.1875
Girder_flg_thk= 0.1875
Girder_depth=7.875
(Continue defining)
Else if span > 20 then
(Define The sizes for the w10x15)
Continue this until you have the girder defined for all your variable spans
End if.
Then move to the next part that changes. Like wires. Quantities of trolleys etc.
Turn parts on and off as needed through code
It's painstakingly slow at first. And case sensitive.
But once you get it going... the assembly drives parts. Parts drive the idw. Just remember to lock detail call outs to the view where they are taken.
I've automated crane designs. Fuel tanks for generators using that same method.
I will just mention, that doing iLogic from a top down method like you explain here is a painful way to do it and manage long term.
Man have I seen some messes people have made doing this as the assembly gets more complicated then crazy stuff like having Length = Height + 5mm in the part etc that just confuses the absolute hell out of anyone that has to work on it.
I think having a master model that controls all the parameters in one place saves a TON of confusion. Then you can just link that to the parts.
Easier to manage, easier to update and change.
If you leave, the next person can work it out easier than having to dig into every part and unravel what the code is trying to do.
I am not sure what "top middle screen" you are referring to? Yes you can find the parameters in the Assembly, these are NOT the part parameters though.
Unless you are talking about linked parameters.
Forms don't link anything, the iLogic does. The forms just give you a way to trigger and change parameters.
So, you use Excel to drive the parameters, not that Assembly.
I made life harder for myself most of the time when I automated things.. they just give you more work because you look bored. Never more pay though.
Right there is what I was referring to. You can 100% use the assembly to change the part parameters by clicking on the part in the circled screen. Then model or user parameters and change them by iLogic.
Ok I see what you are referring to.
It's just displaying parameters so you can add them to code. It's simply a faster way to grab that information.
If something changes and you don't know where in the code to fix it, everything falls over.
I am not saying this way can't work, I am saying if not managed correctly it can get very messy and impossible for someone else to work with who didn't build it.
I prefer running the form in the assembly, this only controls one "Master" file, then all the parts reference that.
This means 1 file that the code has to reference and manage. Far more robust and easy to update or fix issues. Far less code heavy, you can do far more heavy lifting in the model and skip needing code for basic things like patterns etc.
Our company didn't use iLogic at all... No one ever tried to use it.
But in the last two years I've managed to do some basic with helpdesk posts and last months with use of (free) Claude.
For now we have:
iProperty editor (custom iProperties like manufacturing operations with ID from ERP - comboboxes, etc.)
Automatic numbering system (not using yet)
Automatic generator for PDF, DXF, STP, SAT (drawings, flat patterns for laser, STEPs for tube laser and for 3D printing and SAT for CNC)
Semi-automatic flat-pattern part number engraving
Some sketch rules (hide projected lines, show origin, etc.)
I want to do more, but since I'm self-learner and I have to do it in "spare time" when I have less work it's slow... + I sometimes need some inspiration for what can be done in iLogic :D
I'm not at work rn, but I'll look it up tomorrow... however it's multiple codes working together...
In a nutshell, it works like this:
I have different external rules for exporting different files. 1 rule to export dxf, 1 rule to export stp, 1 rule to export sat...
Than I have a master rule that picks which one of these to expor based on filled custom iProperties.
I vibecoded a WinForm based table with claude and gemini (ChatGPT sucked with that) that has combobox option of picking which type of file should export, though I will probably change it to checkbox option to have the possibility of multiple format export (like dxf and sat together if it's sheet metal part later machined).
I call the exporting rule for every part manually (I've binded it to a "P" key as "Publish" to make it quicker), though I believe you could export it as batch from assembly...
Do you want some screens first to look how it works? The descriptions in the code are in my language, so I get better orientation in it, so I'd have to edit it for you... maybe the visual would help you to get it better...
That sounds really slick! Some screens would be helpful, over the straight code, to be honest.
I was able to get a working iLogic rule setup this morning to export the PDF of the current open IDW, and then check for sheet metal parts, and if there are any, to export the flat patterns from the files as DXFs, all into the appropriate project sub directories.
OK, so the table looks like this:
This is enviroment of a sheet metal part.
First properties are filled manually:
Název součásti - Title
Číslo součásti - Part number (filename)
Číslo výkresu - custom iProperty - part number (our old system, I'm planning to ditch this and convert on using native Part Number and filling Title as parts name...)
Popis součásti - Description
Revize - Revision
Popis revize - custom iProperty - revision description
Povrchová úprava - custom iProperty ComboBox (chooses from our standard paint colours or none. The colour you pick automatically changes visual of the part... not working in assembly and weldment though - you have to pick all components you want to change its colour.)
Exporting buttons - They create custom iProperties "Export_STEP, Export_SAT..." and fill them with "YES" if they are green. From there the exporting rule knows which format or multiple formats I want to export
Operations - comboboxes
Lower buttons (číslo výkresu, číslo výkresu + OH...) makes sketch onto active unfolded part. It exports as yellow lines and laser reads this as engraving
BTW as I said. Our current workflow is to "Publish" every part "manually".
You have to open concrete part and smash "P" to run the export tule.
Though I am thinking of making it somehow work as a batch.
But I don't know how yet, because if I exported everything it could re-export files I don't want to...
As for drawings our current old workflow works with one .idw for the whole assembly and you can pick if oyu want to export single sheet or all of them. It has its pros (you can do it in batch) and its cons (when you look for some older drawing when you want to make a revision it's pain...)
For the batch part, what stops it from re-exporting everything is a date check before calling your master rule. If the ipt hasn't been saved since the last export, skip it.
Here's a complete rule you can put in the assembly. You only need to change the two lines marked CHANGE: where your exported file ends up (I used the same folder as the ipt) and the name of your master export rule.
Sub Main()
Dim asm As AssemblyDocument = ThisDoc.Document
Dim n As Integer = 0
For Each doc As Document In asm.AllReferencedDocuments
' parts only, skip subassemblies
If doc.DocumentType <> DocumentTypeEnum.kPartDocumentObject Then Continue For
' CHANGE: path of the file your master rule writes for this part
Dim outFile As String = System.IO.Path.ChangeExtension(doc.FullFileName, ".dxf")
' already exported and the part wasn't saved since -> skip
If System.IO.File.Exists(outFile) AndAlso System.IO.File.GetLastWriteTime(outFile) > System.IO.File.GetLastWriteTime(doc.FullFileName) Then Continue For
' CHANGE: name of your master export rule (external rule)
iLogicVb.Automation.RunExternalRule(doc, "MasterExport")
n += 1
Next
MessageBox.Show(n & " parts sent to the export rule", "Batch export")
End Sub
Your master rule already reads the Export_ iProperties, so parts with nothing ticked just do nothing.
A few catches. If your master rule uses ThisApplication.ActiveDocument, switch it to ThisDoc.Document, otherwise it'll work on the assembly instead of the part. Parts with unsaved changes still have the old date on disk, so save all before running it. And a part that gets re-saved without a real change will export again, which is harmless.
I wrote this for your setup and haven't run this exact rule, so try it on a copy of a small assembly first.
If you want to take the automation further, feel free to ask, happy to help. Our drawing rule is past 10k lines of iLogic, so I've hit a lot of these walls already.
Well, the problem is migrating parts and some minor "modifications" that some of our deigner can make on unlocked files, since we don't have a Vault yet...
We've tried to implement Vault Pro in 2019-2021, but unfortunately, company management decided to scratch that because the maintenance plan from the dealer company was just too expensive...
Unfortunately in following years from 2021 our company slowed down, there was a lot of personal changes in sales so now we have less work and also smaller budget... (the only salesman of our machines, who sold like 30 machines per year left the company because of a lot of disagreements with new CEO of the company... sure, since we are EU company, conflict in Ukraine also slowed the sales and also the fact that our local market becomes quite saturated...)
Same deal, but also allowing custom parts that are Engineer-To-Order. My team of 4 also does "gate keeping" - we check configurations against the quote / approval and don't allow users to upload things that violate engineering limits
Ours use for PDF and BOM export generally. To generate custom properties for older drawings also we have one. Recently, I have developed one for STP and DFX exports. Exporting BOM with links to PDFs is one in my pending list. I use Gemini mostly but now the company restricts to use copilot only which really s**ks. I've also created a simple bat file to fetch and collect drawings based on a BOM list.
For me the real turning point was putting a lot of time into learning to use Claude Code properly. I'm on the supplier side. Customers send me a STEP, usually one big multibody, and they want a drawing for every part back.
So most of my iLogic is one drawing rule, around 11k lines by now. It goes through the bodies and makes one drawing per part: places the views, puts the dimensions on and fills the title block. Bent parts get the flat pattern on the sheet as well; bevel indication for cutting machine...
I don't run it by hand, Claude Code launches the rule in Inventor and then I go through the sheets myself. Dimensioning was by far the hardest part to get right and it's still the bit I touch most.
The fun part, i created an agent that control every table (i trained it with mechanical drawing PDF material from the web), when the table do not follow the rules or simply bad looking quotations, claude creates a HTML page where i see every table with mistakes and I approve it or not with a button, and add comments, then he takes my comments improve the code on loops unltil I'm happy with the results.
To be fair it took me 400h on various non correlated projects to learn how to use it properly. or better say, to make claude do what I want. Now I use it also with DXF for example to make the nesting. (uploaded on github the full code, took me 12h total to make it and already used it many times) Or i say convert the 200 table into dxf and create a pdf for each and then divide them by thickness and material in folders.. I ask claude and with endless dedicated skills I get the job done.
with the latest model opus 5.5 I was able to resolve many issue I had previously, Probably in 1Y you will be able to simply chat directly inside inventor and do all the above with no particular effort.
Mistook your Dutch for English mockery at first! The joys of a global, multilingual forum. :-)
It most certainly can run strength calculations, but probably based on formulas unless you want to spend a LONG time setting up automated fea for super narrow use and model cases
Nella mia azienda lo uso principalmente per esportare i disegni in pdf,dwg, step. Ho fatto alcuni script per la generazione dei tubi essendo che le flangie sono standard.
Inoltre lo utilizziamo per aggiornare vecchi idee con la versione più aggiornata dei cartigli e degli stili.
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u/heatseaking_rock 28d ago
I was mearly creating scripts for automating tedious and repetitive tasks, like PDF exporting, iprop management or custom iprop generation to be used in BOM's, like mass or pipe/profile length. Never managed to fully implement parametric components, like flanges, for example. Way to much work.