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,

ADS.

photo credit: fittings (license)

Work Features

This is first on a three post series where we cover publishing dumb parts to content center. Consider dumb parts any featureless models you download from the internet. While some download servers will give you Inventor models with features they have no dimensions and no parameters, in short, they are still dumb. On my last post I gave you a couple of websites where you can download models and increase your content library and if you’ve missed it then you can read all about it here.

Some of my parts have just as many work features.

Before we discuss how to create a family of dumb parts and publish it to content center I need to make sure that you understand a couple of things like how to create work features. While you probably have this nailed down I will take some time and show you some tricks on creating work features. These are especially needed if you are going to publish tube and pipe fittings to content center which we will cover in the last post of this series.

You can create your work feature backwards in a reverse order and as long as you remember the sequence you can go back as much as you like. Start the work feature and then right click and choose plane, axis, point which will pause the action and start another sub-feature which will serve as the input for the first one in an endless loop which will consume inputs nesting features one under another like Russian wooden dolls.

Nested workfeatures are like russian dolls.

Let’s try this out see just what I am talking about. In the vessel below I need to have an exact minimum dimension from the top of the nozzle to the tank. The tank is a dished end stainless steel vessel and it’s not as easy as constraining the face of the nozzle in regards to the tank surface, especially since I need this to be calculated automatically when I change size and position (angle, or pcd) of the nozzle. For faster/better results I am driving all the connection with ilogic and forms so it makes sense to have the minimum distance calculated automatically.

Min. nozzle dimension for clamping and access.

The cut for the nozzle was done on a planar sketch because we need the nozzles parallel to the ground rather than perpendicular to the dished end surface.

In the planar sketch I have defined a point on the tank center side of the nozzle cutout circle which will always give me smallest positional distance but in order to use this point, the sketch needs to be visible.

Getting the minimum distance point

Normally you would:

- Start work axis command, and choose the point and the base plane.

- Start a work point command and choose the previous axis and the dish end outside surface.

- Start a work plane and choose the previous work point and the base plane. Alternatively you could select the point and the axis.

Usual way of creating workfeatures.

Now you have a work plane which can be used to constrain your nozzle face against. You have to restart the command 2 times before you get to the end and while you can have it on auto-repeat I will now show you how to do that in one operation. You also need to turn off the visibility off for all these work features because they are not off by default as on the method I will show you next.

TIP: When you start a work feature command you can right click and choose “Repeat command” which will keep the create feature active when you finish doing one but to end it you need to right click and choose Cancel or press the Escape key. You can also press Spacebar or Enter to repeat last command just like in AutoCAD.

 

Right click for extended menu.

Let’s do this in reverse with a single command. I will do arrange it in a tab formatting for better visual understanding on how this works:

1 - Start the work plane command (that’s the end feature we’re after)

                A – For the first plane input right click and choose work point

                                o – For the first work point input right click and choose work axis

> - Select the sketch point as the first input of the work axis

> -Select the sketch for the planar direction (or the base plane)

                                o – Click on the dished end outside surface as the second work point input.

                A – Click the base plane (or the axis again) as the second input of the work plane.

 

Faster way of doing the workfeatures.

                So now you have same work plane but the sub-features are hidden already. This is a nice trick but for many sub-features it can be daunting to remember the whole sequence.

             

Too many workfeatures in reverse can be daunting to create.

                Next time I will show you how to author empty parts as tube and pipe fittings so you can do your routing without knowing/having the final design for the fittings.

                Later,

                ADS

Photo credit:

Adivina donde estoy... , (license)
Topless grumpy , (license)
5098 Matryoshka , (license)