how can i make a template that generates parts?

[gregwJ5J85]

basically i have to make a series of assemblies that vary is some minor ways that change the shape of some of the parts, how do i create a template so i can just input those variables and have it give me the parts needed? one at a time would be fine, but i don't want to have to make a whole new assembly where the angle of something changes so i have to manually adjust each part to match. i hope that makes sense.

the part is a pipe support and the angle it makes with the ground is the main thing that changes (between 9 and 30 degrees), but there are several parts that make up the base that change if you change that angle 

originally i thought i could just make the assembly and cut it, but the cut doesn't affect the original part files so a coworker had this idea, but i don't know how to do it

[pcrawley]

iCopy

It takes a bit of figuring out, but it is perfect for that task.  You can build an assembly and then use iCopy to place one (or multiple copies) along some guide rails.  The guide rails control the geometry within the assembly.  Each assembly is built under a unique name, and you can specify which parts are copied and which are unique for that point on the path(s).

There are several tutorials available if you search "inventor icopy".

[Curtis_Waguespack]

Hi @gregwJ5J85 

You could set up a template assembly with some iLogic to do this. See the simple Inventor 2020 assembly attached here for a quick example. I'm certain your designs are more complex than this, but this example might give you some ideas.

I hope this helps.
Best of luck to you in all of your Inventor pursuits,
Curtis
http://inventortrenches.blogspot.com
 

[johnsonshiue]

Hi! I believe iLogic will help in this case. Please share a small example. The forum experts can help propose good solutions. Or, you can google the terms "Autodesk Inventor iLogic configure parts." There should be plenty of examples to check out.

Many thanks!

[mcgyvr]

Can you show an example?

Is it just the constraints of the assembly that change? Or are there actually different parts that are required?

In the "real world" is this support bracket the exact same part number you just bend it or something differently?

A little more detail/example of what specifically needs to change/happen will likely yield you a better solution.. 

While ilogic is very powerful I would always recommend avoiding "coding/programming" when out of the box solutions may be available just to help in the future should your staff not be programmers.. 

Also please state which version of Inventor you have..

You may be able to use model states or ipart/iassembly functionality to achieve the end goal.

[Curtis_Waguespack]

---

@mcgyvr wrote:

While ilogic is very powerful I would always recommend avoiding "coding/programming" when out of the box solutions may be available just to help in the future should your staff not be programmers.. 

---

Just for clarification, for this type of configuration there would likely be no real programming involved. We can use the built in iLogic tools to generate any code needed from the model... and do so in a way that any Inventor user can master in a very short time. I suspect the code involved would be quite minimal.

The distinction here is "iLogic" without "API" (which I've certainly helped muddy the waters on over the years 🙃 )

But in general I agree with all you've said, and would welcome seeing an example as well.

[gregwJ5J85]

it's a pipe support, so it's a base, then i do an angled extrusion to cut where the pipe clamp will sit, that's the angle that changes, so it affects most of the base and the height that extrusion meets each part is completely dependant on the angle. i do have a way i'm going to do it that's better than manually one at a time, but only barely, so i'm still looking for a better method if one exists

also i'm using inventor 2020

[mcgyvr]

A picture or the actual ipt file and a description of which parameter changes would be a bit more helpful BUT.. From what I'm understanding so far you could achieve what you want with an ipart. Each member of the ipart would have this modified angle feature as required.. You could then have and iassembly (if needed) that would swap out the required ipart member as needed. 

ipart help page

https://knowledge.autodesk.com/support/inventor/learn-explore/caas/CloudHelp/cloudhelp/2020/ENU/Inve...

iassembly help page

https://knowledge.autodesk.com/support/inventor/learn-explore/caas/CloudHelp/cloudhelp/2020/ENU/Inve...

[A.Acheson]

Here is a few examples. This is possible in many ways as everyone has mentioned. Some of it will come down to how convenient it is for assembly renaming and file management etc.

Examples attached:

1. Assembly with custom ipart pipe:

File Management:

You need to save the assembly first, custom iPart when changed creates a new file the default file location is in the root of the project .ipj file and not the immediate folder the assembly is in, so you will need to change this path each time. For every custom change to the  iPart  a new file is created so if you are measuring and adjusting 10 times you get 10 files of which only 1 you will want to keep. 

2. iLogic assembly: 

A form can be used for quick access to parameters. You can swap components if required. 

Using ilogic place component you can place a new assembly and you can change parameter values before placement.

Generic indexing is used for both file naming of custom part /assembly so no up front file naming required allowing quicker mock up's. You will likely need changing later as it uses the occurrence name/browser name and an index number 01-02.

Tip:

Using iparts/iassemblies to avoid creating duplicate custom parts when they are likely standardized.

File Management:

One set of custom files is created, 1 for custom assembly and 1 for custom part ( non ipart/iassembly file)

If adjustments are needed only one file requires access and so no new files are created. 

Files are saved in the same folder as the assembly. No opportunity to change file names, these will need to be changed through normal methods.