Thursday, 28 January 2016

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?


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

Monday, 25 January 2016

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.



Wednesday, 20 January 2016

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.



Photo credit:

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

Thursday, 14 January 2016

Content Library

I’ve got a really nice post on authoring dumb parts to Content Center and furthermore, specific to my case author them as tube and pipe elements. This will have to be split on 3 separate blogs because there is a lot of info I need to make sure you all grasp some basic concepts until we jump on the main idea.

I consider dumb parts, anything that I download off the internet and I don’t bother creating from scratch because I lack the time or there is not enough information on the manufacturer’s website.

This is really a prequel to the 3 posts and for now I will give you some websites I go to when in search for 3D parts.

Having a library at hand can save you a lot of time.
 First stop is the manufacturer’s website. There are a lot of manufacturers that provide CAD library straight from their website were you search for the part by item number, size or characteristics and some websites even give you the complete library. Georg Fischer for example lets you download the whole set split into several zipped files based on material ABS, UPVC, etc.

One of my long time favourites is Cadenas Part Solutions.  They are more than a library of online parts but the library is free, intuitive, and when downloading parts in Inventor format you actually get featured parts and assemblies rather than dumb models. The sketches have no dimensions and there are no parameters in the parts but you do get iproperties. I doubt you will be using the default values, but that’s for you do decide. Parts can be added to a download center where you can choose to save them all as zip,have them by mail or even better it has cad integration and it will insert the models in Inventor for you (be careful of the save location). Even better you can set the level of detail of parts and get simplified parts if system resources are low. There is no user content, everything seems to be accurate and I never had any issues like interferences or mismatched models. Parts are configurable and on things like cylinders you can specify the stroke to be generated with.

Cadenas gives you true inventor files.

Several level of details and file format to choose from .
Traceparts has a nice and clean interface but the search engine needs improving. Searching for “brass valve” will give you a mixed result of anything containing brass and anything containing valves. Furthermore not everything is 3d/2d and in some cases you only get a link or just documents but personally I go to manufacturer’s website for documents. You can add parts to” download center” and download them all in a single zipped file but every time I tried more than half a dozen or so I got an error, all files were removed and I had to start over. Downloading all members of a single valve family had to be done in separate batches.
TraceParts library
Thomasnet I haven’t used in a long time and it’s because you get a lot of documents, manuals, and manufacturer’s info and that’s not what we’re after even though you get cad integration and several cad formats to choose from.
ThomasNet library.
3DModelSpace is more of a links database to the manufacturers cad website but you do get a PTC/Creo Standard Parts Library.
3D Model Space
3DContentCentral is part of 3DS (SolidWorks, Catia, Simulia etc.) and even though you can get complete parametric families there are kind of useless in Inventor. The website has custom user generated files as well as supplier certified libraries.
3D Content Central.
 GrabCAD is user generated content only, so I use it as a last resort if I can’t find the part elsewhere I search for similar parts or similar model parts. You get all sort of things here from starwars models to fully modelled engines, guns and spaceships. This is where you come to download car models and render them to you school project or download models created by others to learn some new techniques.
Lamborghini or Audi A8?

McMaster-Carr is more of a sales website but you get a lot of good quality models. And the same goes for RS.
For machine components I go to Elesa, for castors to Blickle or Tente

The websites are in no particular order and as mentioned you should start with the manufacturer’s webpage like:
Georg Fischer

When you open inventor, in the Tools tab, Web pane if you click on Supplier Content you will get a list of libraries on the net but we’ve mentioned them already.
Default Inventor links

I feel I am just scratching the surface with this list and google is your friend really but do share your preferred web libraries on the comments area.