How to create a single part with left and right configurations

[kmoreau48]

Good morning,

I am having problems trying to create a single part file that includes a left and right configuration that I can switch in an assembly. I found a way to do what I want (which is not super user-friendly to use) but I create an ipart table with two configuration where I can suppress the mirror feature from one of the configuration (see screen cast link in order to understand my point)

My problem now is that the reference sketches disappear once I insert the part into an assembly. Is there a better way to achieve this goal and also keep the sketch visible in an assembly?

I was not able to insert my part as an attachment, so here is a link do download it: https://www.dropbox.com/s/c6bvsrz8levhlh8/LD0700_SLB7_Contreventement%20Diagonal%207-0_REV-0.ipt?dl=...

[SBix26]

I routinely create left & right hand parts as separate solid bodies (one the mirror of the other) in one master part file, then derive the solid bodies separately to two individual parts, each with its own part number, description, etc.  This creates three separate part files, but so does your iPart (factory + 2 "configurations").

The advantages of this method are:

• It is very easy to edit the master part and all derived parts follow
• Features can be easily added to both parts (above the mirror feature in the browser) or to each part alone (below the mirror feature)

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Sam B
Inventor Pro 2020.1.1 | Windows 7 SP1
LinkedIn

[kmoreau48]

Thank you for your answer, I am not sure if this workflow will work for me since both left and right parts are actually the same (the two connection points can rotate) so I need them to have the same part number and properties in order to show up as the same part in my part list. Is that possible to do using your method?

[SBix26]

Sure.  The two derived parts have separate iProperties, of course, but the Part Number and Description properties can be the same if needed.

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Sam B
Inventor Pro 2020.1.1 | Windows 7 SP1
LinkedIn

[IgorMir]

Try iParts. Once you finalize your model for, say, Right Hand version - create an iPart, mirror the whole solid with the suppress  origin checked in the Mirror DB. In the iPart Author Table - for the first entry - suppress that last mirror. Add to the table all the info you need from iProperties, edit them as needed and you are done.

Cheers,

Igor. 

[kmoreau48]

That is exactly what I did, but my problem is that once I place the ipart in an assembly, I lose my reference sketch and I need that sketch in order to mate / constrain my ipart to the assembly.

Any idea how I can keep that sketch using ipart?

[rhasell]

Hi

My workflow is the same as @SBix26 , but if you prefer to use iParts try the following.

Create Workpoints / workplanes etc. These can be used for the assembly constraints instead of the reference sketch.

[kmoreau48]

I used to apply constrains using an axis and 2 work planes. I am currently assembling hundreds of scaffolding and I am trying to lower the amount of clicks it takes me to assemble the parts together. I found that "joint" can replace the 3 constrains required into only one joint. That's why I need that sketch in order to use the end point for the joint feature instead of using the 3 constrains method.

But if you look at my screen cast, even the work plane disappear once the part is inserted in an assembly.

I also wish there was a quick left / right button instead of editing an ipart or replace the component if I end up using your workflow

[kmoreau48]

Update: I found two work around for my situation

1. using iparts, instead of using a line and a point in order to "joint", I made a small cylindrical extrusion and I can now apply the joint feature

2. using representation, I mirror the component by keeping the original. I then create two representation (left and right) and hide the bodies accordingly. What I don't like about this solution is when I change the representation in the assembly, the default option is "master" instead of the actual representation shown in the assembly at the moment.

If anyone has a better solution please let me know

[Anonymous]

I did scaffolding in "another CAD-world". There you could create sketched patterns that served as placeholder. I only assembled the basic elements and then patterned the stuff around, in all X, Y and Z. In IV you could mimic this by putting dummy parts in the assembly with patterned features. A workaround to get a component multiplied. Saves on assembly time. Dummy parts can be made invisible.

[mcgyvr]

I would have directed you to create that as parts and an assembly (because thats what it really is).

Then set that assembly as "purchased" so that it acts like a single part in BOM's..

Then create positional representations to create the left and right configurations..

[joseph.hoermann]

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@mcgyvr wrote:

I would have directed you to create that as parts and an assembly (because thats what it really is).

Then set that assembly as "purchased" so that it acts like a single part in BOM's..

Then create positional representations to create the left and right configurations..

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@kmoreau48 I would agree with @mcgyvr here. After looking at what you are trying to accomplish, especially within the context of wanting to use joint behavior, I think Positional view representations with a "Purchased" assembly would be a quick solution to the LH/RH issue here. 

In addition, using a derived part of the original then making it appear as a "ghost" ghost entry in the BOM could also be a potential solution. Please mark this solution as solved if you don't have any additional questions. Thank you!

[kmoreau48]

I will give this a try and see if it works well!!

[Anonymous]

Have a difficulty understanding that you start by saying you need a left and a right part and then state in a reply that "since both left and right parts are actually the same". If they are oriented you need 2 parts. If only the orientation changes for each use then this is something that assembly should take care off.

[kmoreau48]

Basically, the actual part is an assembly of one tube with two connectors. But that assembly has a unique number, whether I use it on one site or the other. The reason why I try to keep it as a part is because I have a library of parts that I use to build scaffolding and I don't want to have to deal with 3 parts + 1 assembly for this case. It does not involve manufacturing, it's only a representation that I use in multiple assemblies. It's easier for me to deal with it as a part even if it's actually an assembly.

[Anonymous]

You can put the assembly in a derived part. It (the derived part) will then behave as a single part. You keep all relevant information and updates because you can 'dig into' the part till you find the components.