detailing weldment parts

[dreadservices]

Question, in Solidworks when detailing a weldment you can add anything to model and then pick parts for detailing, whether it be a gusset, bracket , padeye etc. In inventor I’ve always created an assembly when I’ve been designing a framework, creating components and adding them to assembly, is there a way within Inventor that does the same as SW. See below for example. I want to pick the rolled plate as a part within the assembly drawing, in SW when you start drawing/view you can pick the part and place in drawing, is this possible in Inventor?

[Gabriel_Watson]

You can specify which file (another one) is going to be used as the source for a new Base view window:

[dreadservices]

Got it, but does Inventor have the same functions as SW when creating parts within assembly. A wee bit of pain when creating weldment assemblies. Here’s me sticking up for SW after using Autodesk products for over 35 years😊. Like all software there’s good and bad.

[dreadservices]

Got it, but does Inventor have the same functions as SW when creating parts within assembly. A wee bit of  pain when creating weldment assemblies. Here’s  me sticking up for SW after using Autodesk products for over 35 years😊. Like all software there’s good and bad.

[Gabriel_Watson]

I'm not sure about the exact same tools as SW, of course, as it has been a while since I opened SW to try anything there. However, you can also add new parts into a weldment in Inv. I'm not sure what other tools are you looking for:

[blandb]

Are you using the "weldment" assembly, or just a regular assembly? If using the weldment assembly when placed, you can choose the "model" tab on the base view to decide what you want to show:

• Assy only (no welding, machining, preps)
• Machining (shows the machining operations)
• Welds
• Preparations (allows you to choose each member to detail out the preparations)

This will allow you to place the main assy multiple times, but get different info out of it.

If just using the regular assembly, then as @Gabriel_Watson mentioned, just place in the part needed to be detailed. Others may choose to use design views of the assembly to isolate the components needed, but its up to you. Just some thoughts.

[jtylerbc]

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@dreadservices wrote:

Got it, but does Inventor have the same functions as SW when creating parts within assembly. A wee bit of  pain when creating weldment assemblies. Here’s  me sticking up for SW after using Autodesk products for over 35 years😊. Like all software there’s good and bad.

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For weldments only, this functionality does exist.  On the Model State tab, pick "Preparation".  This will enable a dropdown list that lets you either show the entire assembly or individual parts.

Personally I don't use this feature, but mostly just because we have some automation that relies on the views being placed from the parts instead of the Preparation stage of the assembly.  

[johnsonshiue · Accepted solution]

Hi! I believe you are talking about local components in an assembly all in one document. SWX does support it but Inventor does not. In Inventor, each assembly (iam) references individual parts (ipt).

The only local components Inventor can create are virtual components (component definition without a shape) or AnyCAD linked files (associative import).

Many thanks!

[paul.hadleyEBN96 · Accepted solution]

SW has a great feature in that you can do multi body welded parts, unfortunately with Inventor you have to push the part into an assembly and then add the weld elements at the assembly level. Crazy I know, a lesson on how to make things difficult when it shouldn't be!

[johnsonshiue · Accepted solution]

Hi Paul,

The concept of a part is relatively strict in Inventor compared to SWX. A part is the lowest denominator like an individual part in real world. It has the geometric definition for the part only. Though you could build multi-solid body part mimicking an assembly, it is for shape definition only. You still need to push individual bodies as parts in an assembly.

There are advantages and disadvantages. Regardless, it does not block you from getting the job done.

Many thanks!