Fitting Engagement Distance

This has been in my drafts way to long. I only allowed myself to publish new posts if there is one ready to go in my drafts. Even though I am not back to normal I feel this might help me move towards normality even if I might never get there again.


Can fittings have both male/female connections and different engagement distance?

My friend asking this was referring to elements like bushings, and reducers as in the image bellow where the right side connection can fit 2 sizes, one inside (female) and one outside (male). These will need different engagement distances as well.

3 connections on same fitting.

Library or stand alone?

There is no gender on the fittings; they are all connected by points and axes but how you author it depends on what you intend to do with the file. Is this for an ipart to be published to Content Center, or is it a standalone library file?

More than likely this will be used in content center but if this is a standalone library then you need to author this in a weird way with 3 connections instead of 2. When you place the fitting press Spacebar until it shows the correct position.

While this is possible I think most of you will need this in Content Center. For that you will create two identical shape members with different connections.

Even though these members will have identical part number, stock number and whatever fields you use to identify this, the filename needs to be unique. This is one rare occasion when I allow filename to be different than the part number.

How do we create a dynamic engagement distance? You create an offset work plane and you control the offset value from the ipart table.

 

offset plane

 

ipart table

In the author fitting window choose Engagement, To Plane, Point and choose our plane.

 

Authoring, To Plane / Point

Later,

ADS.

photo credit: parts (license)

Publishing Dumb Parts

This is last part of the series, covering how to publish dumb parts to Content Center. Now you know where to get parts on the internet, how to create work features, and how to author empty parts. This is all neded info before we take the final step.

                Quite simply publishing dumb parts as a family in content center is based on the ability to create iparts with suppressed bodies (will expand later).

Downloaded parts can stay dumb, we'll make them smart.

                As you probably know if you follow this blog when I download parts from the internet I don’t publish them to content center but I keep them in a library folder and the document properties are saved in a text file. When I need to place a certain valve I copy the file path from the text document, and I paste it in the place fitting dialog window to speed up my navigation time. Content center seems slow as it is and I don't want to overload it with individual parts.

                While placing from disk is faster than placing from content center (it is for me) there is another limitation that we can’t overcome. Insert fittings only seems to work with content center items, parametric or dumb all the same. If you don’t know what I just said I suggest you get familiar with my blog on inserting fittings here.

Placing fittings will insert nodes on the route which breaks constraints and remove dimensions. A better way would be to place the main fitting say a valve and insert the rest of the fittings before and after, like reducers, unions, etc. This way you only need to control the position of one node on the route and the sketch remains fully constrained. Insert fittings only works with content center items and to overcome this you would first need to place a CC item and then drop your library item (located on disk) over that CC item. These are way to many steps, so for this we will publish them to CC as a family.

I am going to use a Georg Fischer valve set as an example.

TIP: You can download the whole Georg Fischer cad files as zipped packages split by material type, ABS, PVC-U, PVDF, etc.

Georg Fischer metering valve as example.

I needed a metering Valve so, to replicate my case,  after locating the stp files start a new assembly in Inventor. Drag the step files inside the graphical window of the new assembly. If the files are computer generated then the origin will match for every single one of them even though when they are dropped in the assembly they will be automatically positioned at certain distance from one another. You need to position them on a common origin, and even better to the origin of the assembly. Use the Assemble tab, Productivity pane, Ground and Root Component command to fix them at the origin really quick. As you can see in the screenshot I have GR as my speed key and that helps a lot.

TIP: The files will be imported as per the last Options you chose for this particular foreign file extension. If they are being imported as composite surfaces rather than parts with bodies read down towards the end how to change the import options.
 

Use Ground and Root Component to fix them at origin.

This is a perfect example because with 2 models we are going to cover 4 members in content center. Because the models are the same there is no point getting all 4 stp files and only 2 will do. The other 2 models are identical having different part number due to different gasket materials.

If the models had a common origin you should see them overlapping just like on my section in the image bellow. If not you will have to constrain them to a common origin, and then to the assembly origin.

Locate imports on a common assembly origin.

The next step is to get this assembly as a single multi-body part because for now it’s only parts that can be authored as T&P and parts only that can be published to CC. Derive and Shwrinkwrap didn’t worked in all my tests because the bodies were not coming in as suppressible features. Save the assembly as “stp” because “sat” for all my tests looses the color of the bodies and I don’t want to fix appearances as well. Click open and browse to the new stp. location.  You might need to change the file extension filter to Step or Any (*) and select your file. Click Options next to Open and then make sure you choose Solids, Assembly as Single Part and Multiple Solid Part. This will allow you to suppress the bodies unlike doing a shrinkwrap or derive.

Shrinkwrap or Derive didn't worked for me.

Use the Options button before Opening the document.

TIP: If you don't get solid bodies on your imports you can play with stitch, sculpt, combine, and get solids out of surface bodies, but we do need bodies for the suppress command.

In the part environment use Parameters and add two parameters, z and L (my case) which will be your connection distance and engagement distance. For butt weld you don’t need an engagement distance. Just like in authoring empty parts we will create work points for our connection reference using work planes located at L/2 on each side and the inline origin axis. As you can see the catalog has no dimensions for z but I have measured the models and added the value to the table.

Missing dimensions can be measured on imported models.

Create connection points using parameters.

Before you click the create ipart button I suggest you rename the bodies in the browser because they will be hard to identify on the ipart table. Here’s my example, and remember that a single body will serve 2 family members. If you don’t do this, in the ipart table you will see “body1”, “body2”, etc. which is hard to locate.

Rename bodies to make easier to identify in the ipart table.

Once finished adding the ipart table info test the model by switching between ipart members and see if the model updates. I have an excel spreadsheet as template for Georg Fischer families and once I’ve clicked on create ipart, I close the table without edits and I open it in excel where it's easier to paste the data from my template which covers, material, description, DN, part number, etc.. and even cost and stock info.

Test your model by switching between components.

Author the ipart as Tube and Pipe component using the connection points created and the “To Plane / Point” option choosing the engagement planes.

Author and publish your part to Content Center

Once you publish this to Content Center you have access to Change Size command but most important the Insert Fitting command.

Insert Fitting is working for CC items.

Keep in mind that adding all these bodies will increase the size of the file a lot and for simple parts you are better off to model it rather than adding them as suppressed bodies which can be a bit of overkill.

Hope you are still with me; I will do a video for this might seem too much to some of you.

For your convenience I have attached the files in a zip document so grab it here and start playing with it.

How do you like my next car?

Later,
ADS.

                

photo credit: stay dumb! glue pinella & DSCF2330 (license)

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

               

Butt Fusion Fittings

Still buried with work and not sure if I’ll be able to do a video but at least you will have some quick info on how to do but fusion fittings and routes in general.

Depending on the complexity and detail you need there are a couple of approaches to take here. The simplest one would be to ignore the discrepancies before and after the pipe welding but you can take it all the way and create your excess welding material as ifeatures that you can drop on each fitting you author.

On my plant layouts I always ignore them because we tend to have plenty of space and discrepancies can be ignored. Quite simply on a 10 meter pipe the assemble tolerance will incorporate any variation from welding or thermal expansion.

So unless you’re into designing medical equipment or any other precise, tight tolerances equipment I would not bother. Keep this as a reference if every once in while you need to do renderings, or the client asks for these welds to be in place and ignore them the rest of the time.

On the simple side, quick and dirty if you do need to have proper, exact cut-to-length dimensions and BOM reports then you need to over-define your engagement dimensions so that the parts interfere therefore reporting correct pipe length and correct route dimensions, node to node.

If you do need to get all that detail exact and you have all the time in the world I would suggest you do the fusion as a ifeature that you can drop on each fitting. Make that ifeature table driven so you can choose and change size on the fly. You can take it down another level and calculate the lost volume from the cutout (melting) and generate your weld bead based on that but that’s way too granular for me.

If you need to author ipart fittings like elbows, tees, or anything else that has a table and might go to Content Center then define new planes driven by the fusion distance and set your engagement to plane/point so you can drive the engagement for each fitting diameter separately.

I recommend that you don’t change or re-author the pipe because you might use that pipe on different connection style (socket welding, jointed, etc.) and it will mess those up. Do all these changes on fittings and it will drive the pipe engagement as well.

Don’t just stop here use the over-engagement on compressed gaskets (thank you Chris Benner for the solution), expansion joints etc.
Here are a couple of links on Fusion Welding, general info and dimensions to help you on the process:
-          Local Head Loss in Polypropylene andPolyethylene Pipeline Joint Welded by Butt Fusion - Ing. Jaroslav VeselskýSupervisor & Prof. Ing. Jan Melichar, CSc.
-          Polyethylene Pipeline Systems - Avoiding ThePitfalls of Fusion Welding - Dr Chris O’Connor

And the post on Autodesk forum that generated this idea.

I have managed to do a video for my youtube friends. Not my best of works, you can hear I am tired and out of focus, apologies for that.

Later,

ADS.