Authoring empty parts

                This was really scheduled to go out on Friday but I was just given a major-major project with strict deadlines and huge penalties on our side for any delay so I had to put in the extra hours and effort to get it moving. I hope I haven’t ruined your weekend by giving you nothing to read on your Sunday coffee or whenever it is that you catch up with the past week news, blogs, forums and CAD news altogether. Helps to start work with a bit of laugh and irony.

Part two on publishing dumb parts is all about authoring empty parts. A lot of the times you don’t have the final model because it’s a complicated part to model, you don’t have enough time or information, you are waiting for a different department to model and certify the part. So meanwhile you do as best you can to overcome this, constraining and moving components around to account for the missing elements.

Empty on all sides

                You might take it a step forward and create a similar shape body or surface outline to guide you as of what the occupied volume is so you can avoid any clashes and interferences when the final model will come in place. This applies to everything from valves to skids and other equipment like heat exchangers for which a model doesn’t exist and it’s in the process of being finalized.

When I am dealing with this type of situations I usually create an empty part, author it as Tube and Pipe to serve me in my routing and drop the final model when ready over it with place fitting command.

TIP: The he assembly replace command will not work and you need to use place fitting instead. With the place fitting command you can drop any T&P authored part on top of a different one to create a replace.

                In my last post here, I’ve shown you how to better/faster create work features and if you haven’t seen it go check it out and then quickly come back because we are going to use that same techniques here.

                In order to author a T&P fitting you need a work point for the connection and an axis for the direction of the engagement. You might need another plane to setup the engagement distance but that depends on the type of connection.

               

                You probably did these points instinctually when authoring T&P fittings although you don’t need to. On an empty part you can’t do without work features but on a model with circular edges you don’t need any work features at all; will have to detail this at a different time.

                If you can’t use the origin planes and axes then you need to create your custom work features and I recommend that you rename then work features in the browser to help you find them on later edits.

TIP: If the directional axis matches one of the origin axis then you don’t need to create them AT ALL. The directional axis doesn’t need to be in line (coincident) with the work point and here’s to prove that:

Add caption

I know there’s nothing fancy here but a lot of people are unaware that you can author empty parts and it’s really the foundation for authoring dumb parts as we will discuss next time.

Later,

ADS

               

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)