Removing phantom fittings

                Although similar with last post I need to share some tips on how to populate a corrupted route again. Last post we discussed how to delete fittings and today we are using the info there to remove fittings and segments that don’t update. 

                This is a scenario that I see a lot and it refers to broken links and updates on the fittings. You modify a route and when you try and update the run you realize that some / all fittings don’t update position and sometimes Inventor creates a complete new set of pipes and fittings ignoring the existing ones.

                I don’t have a case at hand but I will share the one on Autodesk Forum I have been answering and which can be seen here.

               

                As you can see from the images, Inventor decided to keep some segments in place when the route has been changed.

                A different case would be when you need to remove the populated fittings and segments from a route like in this post here.

               

                Just like in my previous post you need to move the fittings and segments outside T&P assembly (promote) and then demote them to a new assembly which can then be deleted.

                The problem is, once you move those fittings you can’t populate the route again. We are technically hiding the elements outside TP and then we delete them so the route has no clue that the parts have been deleted.

                If you do need to populate it again then I have a trick and this is the reason we are here today.

                The route can’t be populated again but you can copy/paste it and then make it adaptive and this will replicate your exact route. Because you are doing this at the route level (instead of run level) you will get the default fittings and not any manually placed ones (valves, reducers, etc.) but nonetheless it is far better than sketching the route again.

                Inventor will NOT place the route in the original location and you will see it at a distance adjacent to the corrupted one.  As a rule any new files will be created at assembly origin and that means that any route will be located at the run origin but without constraints. You can always check the position of the original one by checking the iproperties/occurrences tab.

                You have two options to move the route to a new location:

1                1 - You have not used the Make Adaptive command yet. Once you paste the route you can then right click on it and in the iproperties / Occurrences tab you can enter 0 in the “Current Offset from Parent Assembly Origin” and then click apply. Then you can use the Make Adaptive command.

Position route at origin.

Make Adaptive menu.

                2 - If you have use the Make Adaptive and even used the Populate Route command you can repeat the steps before but in the Occurrences tab take of Adaptive first and then put 0 in the offset value fields. As soon as you click apply, the Adaptive box should be ticked automatically for you if not make sure to put it back. You can't just change the position of an adaptive route or you will get this error:

"

                "Properties: problems encountered while executing this command

                Invalid input for Request"

Take off Adaptivity first.

Limitations:

-          You still need to connect the route to your equipment around.

-          Sometimes, if the location of fittings and segments don’t update you need to edit the route and simply click on “Finish Route” to force an update. Update button or rebuild all will not help you.

Force update the fittings and segments.

Small animation of the process.

This trick is part of the “How to constrain my TP assembly and its components” blog which will come at a later time. Way too many to handle at once.

Latter,

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photo credit: fittings (license)

Linking parameters

                A lot of the times you will need to create matching features (like holes) on different parts. You could create a single sketch and then derive it into separate parts or you could use “Make Layout” on the Layout panel of the Sketch tab, also located in on the Manage tab. This will use sketch blocks or solid bodies but you need to think ahead, and prepare the project beforehand and it will not be covered here. I want to talk to you about all those cases when you would use project geometry while in an assembly to mimic the features of one part into others. While this is fast and well permitted for small assemblies it is not recommended for large assemblies.

                In fact in my Application Options I have stripped out this making sure that adaptivity and associative doesn’t become a memory hog killing Inventor and taking all the fun out.

                TIP: If you hold down CTL wile projecting you will get the opposite of what you settings are. If the settings are set to create adaptive / associative edges then using CTRL you will in fact create non-adaptive / non-associative edges and vice-versa.

                In those rare cases where you just want to copy geometry from one part to the other you still have a lot of options like linking parameters, deriving one’s parameters into the other, copy the features/bodies at the assembly level and all of these options will update automatically for you. 

                But, do you really want it to compute them all the time, when using operations like rebuild all, when opening files, or when you just click update on the quick access?

                What I like to do is derive the parameters of one part into the other, no bodies, no other features, just the parameters and the reason for this is because a derived part can have the option to Suppress the link or Break the link so I can control what gets updated and more important when gets updated.

                TIP: part edges can change with a simple operation like chamfer or fillet and if you rely solely on project geometry with adaptivity you will have broken links and references.

                Give you parameters a name either when dimensioning or by adding them manually in parameters. When the dimension pop-up window shows up you can create custom name parameters dynamically by entering the name with no spaces, just underscore, followed by = and the value you want like this: “Hole_Distance=30”.

stop adjunsting your monitor, the screenshot is not paralel to sketch plane

                When you create a similar part go to 3D Model tab, Insert panel or Create panel and use the Derive button.

                In the settings dialog don’t bring any bodies, expand parameters and tick the ones you need bringing in.

                Now you can dimension your new part and have it update automatically when the original one changes.

                TIP: For coordinated assemblies you should look into linking files with excel which will provide a single source of control for your file updates.

Later,

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