Coming from Solidworks to Inventor - help with using the same part twice

[Anonymous]

Hi,

I am trying to setup some 'templates' in inventor. I want to be able to model the part once then use it as many times as i want but with slight differences such as the length. Much like a dynamic block in ACad.

I have a standard extruded profile. I would like 1 file that sits in a template folder so that when i start new projects i can use it in a new job, without it effecting the 'template' file.

In solidworks, the way i would do this is:

1. Sketch profile
2. Save as template
3. Start a new project / job
4. Use weldments and then i can insert as many as i like at different lengths

How do i go about doing this in inventor?

I know inventor doesnt use weldments or has no feature similar to it.

I think it may have something to do with Parameters. Ive played around with a few things but it doesnt seem to be exactly what im looking for. The end result must be something as follows:

1. Start new project / job (assembly)
2. Place part
3. Use part as many times as i want at different lengths

Hopefully ive made sense. Any help would be appriciated. TIA

[mcgyvr]

You would do that the same way you would in Solidworks..

Create your part (could just be a sketch with the profile or one where the profile has been extruded) then do a file..save copy as.. save as template..

Inventor also has a weldment environment..

https://knowledge.autodesk.com/support/inventor-products/learn-explore/caas/CloudHelp/cloudhelp/2016...

However... I wouldn't do it like that and depending on your needs might use an ipart (similar to solidworks configurations I've heard) and may even use it with frame generator.. 

https://knowledge.autodesk.com/support/inventor-products/learn-explore/caas/CloudHelp/cloudhelp/2014...

Not sure what you are doing but for some reason I think frame generator might be something that interests you too..

http://help.autodesk.com/view/INVNTOR/2018/ENU/?guid=GUID-953F560A-C2D3-4031-8348-762054C7C779

If you are making "frames" of such with this profile then it may help speed up your process there..

You might want to get some training in Inventor and learn what the software can do before you just move forward with what you think is the right direction now (which may not be and may end up costing you time in the future when you figure out you assumed the wrong path to take)

At the very least spend a few hours going through the "learning path" in Inventor and maybe watch some youtube videos..

[Anonymous]

By the sounds of it ipart seems the way to go.

Cant seem to get it working though. I have set parameter "LENGTH" (which is linked to the extrucion dimension) to allow custom values. When i go to an assembly and try to place ilogic component it gives the error cannot be used to place an ipart. Use place command. However that does not let me double click the part and go in to the parts parameters.

Im obviously doing something wrong.

I have done some youtube training but nothing that explains the features properly and how to use them.

[mcgyvr]

Give me a few minutes and I'll whip up a video showing how to use iparts without defining "preset" lengths but instead allowing you to customize it upon placement into an assembly..

hold please 

[JDMather]

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@Anonymous wrote:

....4. Use weldments and then i can insert as many as i like at different lengths

---

Your SolidWorks description is the equivalent of Inventor Frame Generator.

You publish a profile just like in SolidWorks.

[chris]

can you show an image of what shape you are trying to use as a template? iparts as templates are nice, but they have their draw backs... they will not stay active like the SW configuration parts do, you basically have to choose your option and then delete your ipart table, otherwise you will start building a large folder of members.

All my Structural members are set as iLogic templates, this way I can keep the part "live" and change back and forth between sizes WITHOUT building a folder of members to also manage... as I mentioned earlier, iparts work great, but managing members in a Vaulted environment is not a fun task.

I can also show you my method if interested. Also, learn to use your Parameters table, it's very powerful and completely different from the SW workflow... Our company has tried to make the switch to SW twice, but each time iLogic and Parameters keep us from doing so.

[Anonymous]

Maybe im getting confused...

Weldments in SW is basicly structural members and custom profiles.

Weldments in inventor looks like its preparing a part or assembly for welding.

[JDMather]

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@Anonymous wrote:

Maybe im getting confused...

1. Weldments in SW is basicly structural members and custom profiles.

2. Weldments in inventor looks like its preparing a part or assembly for welding.

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1. SolidWorks Weldments = Inventor Frame Generator

2. SolidWorks does Weldments as multi-body solids rather than as the true Assembly that mimics the real world.  Inventor mimics the real world.  You can also do Inventor Weldments as multi-body similar to SolidWorks.

But for structural members you want Frame Generator in Inventor.

Start a new Assembly (an assembly is a collection of parts, just like the real world).

On the Design tab in assembly environment - select Frame Generator.

It is best to first create a skeleton to control the frame (just like in SolidWorks).

[Anonymous]

Attached is an image.

[mcgyvr]

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@Anonymous wrote:

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@Anonymous wrote:

Maybe im getting confused...

1. Weldments in SW is basicly structural members and custom profiles.

2. Weldments in inventor looks like its preparing a part or assembly for welding.

---

1. SolidWorks Weldments = Inventor Frame Generator

2. SolidWorks does Weldments as multi-body solids rather than as the true Assembly that mimics the real world.  Inventor mimics the real world.

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Thanks JD for the explanation... Having never used Solidworks I made some assumptions based on the naming of it.. But for some reason I still felt like frame generator was applicable..

Kind of goofy that SWx calls them weldments..

So yes.. custom profiles to frame generator is the way to go..

https://knowledge.autodesk.com/support/inventor-products/learn-explore/caas/sfdcarticles/sfdcarticles/How-to-publish-custom-profiles-in-Inventor-to-be-used-with-the-Frame-Generator.html

[Anonymous]

Im not trying to make a frame though.

All i want to do is increase or decrease length of an extruded profile on multiple instances in the same assembly

Much like a dynamic block in Acad

[chris]

Yes, Frame Generator is a way to go, but you can also use your own custom parts outside of the generator. The Generator is fast but it forces you to work within it's boundaries. One thing you might also have to "get over" when coming from SW is the idea of designing your "weldment" as on part file.

SW basically teaches multibody modeling for it's weldments... which can be done in IV but is not very user friendly when creating drawings that may or may not have to go to different areas for manufacturing. you can have a weldment made up of several "part" files... after-all the term "weldment"  can mean several things. I personally don't use the FG, I create my individual parts and constrain them together, but as mentioned earlier, I have all my structural members as iLogic templates with coping features already applied... they just have to be (turned on).

[chris]

that will have to be handled with an ipart or a separate part, you can't show the same" file" in two different lengths, but you can have the same part with two different "members"... that have the same part number but different lengths

The dynamic block can do this because there is no "file" associated with it, it's just a series of lines...

[JDMather]

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@Anonymous wrote:

...All i want to do is increase or decrease length of an extruded profile on multiple instances in the same assembly....

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Then iPart is the way to go as suggested earlier.

[chris]

mike, where are you located? 

[Anonymous]

Manchester area.

Ive got myself too confused with it. The only way i can do what i want is:

create profile and extrude.

place in assembly.

double click part which edits in place

go to parameters and change the length

[JDMather]

Attach your *.ipt file here and someone will convert it to an iPart in about 30 seconds.

You can then place the iPart into your assembly with any desired length.

[mcgyvr · Accepted solution]

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@Anonymous wrote:

Im not trying to make a frame though.

All i want to do is increase or decrease length of an extruded profile on multiple instances in the same assembly

Much like a dynamic block in Acad

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Then why the mention/use of weldments in solidworks?

My understanding now is that its for creating frame assemblies like Inventors frame generator..

If you just want to make a normal assembly then just use iparts to achieve your needs..

and here is that video showing how to make a custom length ipart and place it into an assembly..

[Anonymous]

Thanks,

I have managed to get it to work like that.

How come when i create an ipart it makes another folder "OldVersions" and also another part file with "-01" at the end. Its also using this file when i insert into an assembly.

[mcgyvr]

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@Anonymous wrote:

Thanks,

I have managed to get it to work like that.

How come when i create an ipart it makes another folder "OldVersions" and also another part file with "-01" at the end. Its also using this file when i insert into an assembly.

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@Anonymous Inventor always creates an "OldVersions" folder and puts "backup" copies into it each time you save.. The number depends on your project file settings.. a -1 for "Old Versions to Keep On save" means all.. 0 is none.. 1 is one,etc..

That happens for any/all inventor files.. 

edit.. and image showing where that is in your project file settings..

iparts will also (normal ones..not custom parameter ones) create a folder named as the factory and keep all the "members" in it.. iparts are the "factory" file which is the main file that you manage all the versions in.. and the "members" are the individual versions..

You will see that if you create a "normal" ipart factory..