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)

Length parameter format

Those of you working with frame generator or with content center steel shapes know that in order to get the length parameter to display correctly you need to edit the parameter formatting.

So how do we change the content center steel shape template?

Now you have two options:

The first one would be to open the file from Content Center and for that you can click on the big I top left (inventor menu) and in the open flyout menu choose Open from Content Center.

The second option is to edit an already generated file or create one by using place from content center in an assembly.

Once you have the part open you can edit and format the parameter display and then you will need to update family template in content center using this new file.

Let’s detail the first option which seems a bit quicker as well. You need to copy the family first and then generate the file because otherwise Inventor will complain that the new template is not a valid file.

- To copy the content center family to a read-write library like My Library provided by default use the Content Center Editor from the Mange tab, Content Center pane and browser to the family.

- Right click the family and copy it to your library.

- Click on big I top left and from the Open fly-out menu choose Open from Content Center, then choose the family you just copied and in the member window make sure you choose Place as Custom. Length and size it's not important so choose any.

- It will then prompt you for a save location and then will open the file for you. Now you can edit the parameters removing trailing, leading, units, and change precision to suit you.

- Now you need to edit Content Center again with the Manage button and then change from Merged View to your library (THIS IS IMPORTANT) or the extra commands will not be available.

- On the contextual right-click menu choose Replace Family Template and select the file you have edited.

So how about all those files generated already?

 Unfortunately you need to open and edit each and every file individually or use code injector and run this code.

Code injector can be found here and the original ilogic code was posted on the autodesk forum by Curtis Waguespack so head over to the original post and give him kudos.

'-------------start of ilogic code ----------------

'get the parameter
oPL = Parameter.Param("G_L")
'export the paramter as an iProperty
oPL.ExposedAsProperty = True
'set the parameter as a custom property
oFormat=oPL.CustomPropertyFormat
'set the custom iProperty as a text type
oFormat.PropertyType=Inventor.CustomPropertyTypeEnum.kTextPropertyType
'set the precision
oFormat.Precision=Inventor.CustomPropertyPrecisionEnum.kThreeDecimalPlacesPrecision
'set the unit type
oFormat.Units="mm"
'set to show/not show the unit string (use True to show)
oFormat.ShowUnitsString=False
'set to show/not show the trailing zeros (use True to show)
oFormat.ShowTrailingZeros = False
'set to show/not show the leading zeros (use True to show)
oFormat.ShowLeadingZeros = False

'-------------end of ilogic code ----------------

Inventor Assembly Template

                There is a lot of info on the internet on how to setup your template files and many of you have already configured the drawing template, adding title blocks, borders and some symbols maybe. You have probably edited the part template and changed the default material but chances are that you haven’t altered your assembly template too much if at all.

                I am saying this because I see recurring questions popping out every once in while by frustrated people doing repetitive tasks that could have been avoided with a proper setup of their assembly template.

                One of the main things that will save a lot of frustration would be to setup a new design view representation as default instead of the locked “Master”. God knows how many times I’ve found Assemblies that cannot be saved because of the “Main design view is locked” error.

TIP: Instead of locating the template file and folder you can create a new file using New command and then save those changes in the template using Inventor (big I top left) / Save As / Save Copy As Template command.

                So open your standard.iam file template or fire up the new assembly command. Create a new design view representation, I call mine “Default” and set is as active. This will become the default view and hopefully if you don’t manually change it back to Master you should get over that pesky error on editing locked design views.

                The next one up is BOM. By default the Structured tab is disabled and every time you place a Parts List or edit the BOM you need to activate it. You then set it to All Levels, you may change the default delimiter and most certainly you will add and remove columns to suit your design needs.

So why don’t you go ahead and make these changes persistent in the template?

Depending on your design process and needs you might not use this but I recommend that you add Item QTY to your BOM. This will report the cumulated number of instances in the BOM. The default QTY will report the number of items as long as the item doesn’t have a length (G_L parameter) like structural sections, pipes, etc. in which case it will report cumulated length and not the number of items in the assembly.

                I feel better already, anything else?

                I use a lot of Content Center and Purchase Parts that are library read-only items and when doing large assemblies it’s hard to navigate the browser to find that part you want to edit. So what I like to do is add two folders called CC (Content Center) and PP (Purchased Parts) where I group the files to clean up the browser keeping just the normal parts. It makes a huge difference to be able to find something fast not to hunt and pick all the time. Also, you can now suppress hide or disable a whole folder at a time ;)

                Nice... what else?

                How about adding some virtual parts? This is where you get creative and to utilise the tip above you might want to add them to a folder called Virtual. It’s better to add as much you can think off and then delete them in the assembly later if not used. Creative? Like what? Stuff like oil, grease, man hour costs, machining costs, shipment, painting, etc. Remember that you have Estimated Cost on iproperties and virtual parts although exist in the assembly only they do have iproperties just like any other parts. You can even add a long descriptive text in the comments field. Do you need to add the Estimated Cost to BOM? How about Comments then?

                Keep going please!

                 Anything you need changing in the Document Settings? Maybe you want to change the default Lightning Style, maybe not but you might want to change the default dimension display to “Display as expression” to see the full equation driving that dimension. In here you can change the units as well as modelling precision. Verify all the tabs and make sure there’s nothing else that needs changing.

                Is this it?

                On the short list you might also consider:

·         Deactivating the Contact Solver in Inspect Tab

·         Parameters that you keep adding all the time like bounding box dimensions.

·         Link or embed some excel files

·         Add various iLogic Forms if needed

·         Add some iLogic code like one to prompt you to fill in iProperties at first save.

·         Turn on Center of Gravity

·         Etc.

I suggest that every time you find yourself changing settings in an assembly pause and think if this is something that might be saved in the template. If you do this for a week then you’ve probably got most of things but it’s a good exercise to do every once in a while especially with each new Inventor release.

               

Later,

ADS.