Creating a configurable template in OnShape

Step 1 – Determine the part that is going to be made configurable.

This is probably the hardest step to take.  Ideally the part should be one that would be swapped for another.  Additionally, the more parts combined, the more that have to be updated when any change is made to the base part (such as the vendor releasing a new size).  Examples that make sense are bars/shafts/channels offered in different lengths, bearings of different sizes and hubs that have different sizes.  For this example we will use the ServoCity 0.777” Pattern Set Screw Hubs (https://www.servocity.com/770-set-screw-hubs) which are offered in 13 diferent sizes.  Of interest here is that three of the sizes have  hole large enough that the center hub is eliminated from those sizes.

Step 2 – Build a model of the base part that will have some variance.

In this case, we started with the smallest hole part (3mm) and combined the set screw so that we had a single part.  Additionally we out an extruded hole in the center that will vary according to the hub shaft size

Step 3 – Set the document properties

 

Step 4 – To a generic name (no part number) and the URL to the page that covers all the parts.

When there is a higher level page that links to the individual parts (Like the Channels – https://www.servocity.com/structural-components/channel/standard-channel) use the URL for the higher level page.

Step 5 – Also rename the document

Step 6 – To match the same name but also add (Configurable) so that users know it can be changed.

Step 7 – Also rename the tab at the bottom

Step 8 – To the same as the document with the (Configurable)

Step 9 – Select the properties on the generated part

Step 10 – And put in the basic name and description URL.  Note that by putting it in here, it gets propagated in later steps.

Step 11 – Also scroll down and put in the vendor

Step 12 – And click Save

Step 13 – Now it is time to do the configurations.  Find the icon on the right side of the screen that says Configuration panel and click on it.

Step 14 – It will bring up the Configurations panel

Step 15 – In the Configure Part Studio dropdown, select List

Step 16 – A default configuration will be created titled Configuration

Step 17 – Click on the name and rename it to something that corresponds to what makes each part different (Length, Bore, Size).  In this case it is the Bore side.

Step 18 – Click on the field under Name which has Default in it.

 

Step 19 – And enter the first value title.  Note that this should match what the web page for the product calls it.  It does NOT have to be a measurement, it is only a string (which happens to look like a measurement). Hit return when done and it will jump to the next line

Step 20 – Keep filling in the titles until all have been entered.

Step 21 – Next we need to identify what features change with each configuration.  To do this, click on the Configure features button.

Step 22 – OnShape enters a mode where sketches/features can be selected

Step 23 – In this case we want the center hole to be variable, so we click on the sketch to activate it.

Step 24 – Then find the dimension in the sketch which will be variable and click on it.  OnShape will add a new column in the configurations which defaults to the current dimension.  Don’t worry about them all being the same, it gets fixed in a later step

Step 25 – If we want to also make the set screw change position, click on it also.

Step 26 –  In this case it is a translation and we can click on the Y translation value.

 

Step 27 – Which also gets added to the list of configurable items.  Note that this is a good reason why all features should have a good name so that it shows up nicely in the panel.

Step 28 – Notice that the selected value is now outlined with a yellow dotted line.  Now that we are complete, click on the Done button on the yellow box.

Step 29 – This brings us back to the list of configurations.

Step 30 – Click on the first diameter for the Center Hole and change it to the correct value for the part.  Since the Bore title happens to match the size exactly, we can just type in the number.

 

Step 31 – Continue through the list entering the values.  Note that while they LOOK like the strings in the Name column, they are actually values.

While you might be tempted to want to paste all of the items in at once, this is unfortunately a situation where you can only edit a single field at a time.  Sometimes it is easy to have a spreadsheet open with the numbers to be entered and keep switching back and forth copying and pasting into each subsequent field.  Once you get into the swing of it, it is pretty quick to do.  Repeat this for all the columns of configurable data.

Step 32 – In looking at the list, it turned out that one of the numbers was out of order.  To fix, just right click on the row and select Move Up (or Move Down) as appropriate.

Step 33 – Notice that the selected item stays even though it moved positions.

Step 34 – To see the part actually change, just right click on the row and select “Switch to …”

Step 35 – The new row will be activated and the part regenerated with the configured properties.

Step 36 – It is worth rotating the part around so that you can confirm all features are being regenerated properly.

Step 37 – Remembering that we have three special parts, we check them out.  First the 0.500” variant

Step 38 – That looks good, the hub is completely eliminated by the center hole.

Step 39 – Time to check out the 10mm version.  In general it is worth testing the limits of the part to make sure it changes correctly.

 

Step 40 – Unfortunately for the 10mm version, the center lip is still there, so we need to make it go away.

Step 41 -The simplest approach here is to do an extrude from the face

 

Step 42 – Click on the face and create a sketch.

Step 43 – Use the circle around the center hub.  Click on the circle, then right mouse select “Use” from the menu.

 

Step 44 – A black circle will appear corresponding to the circle.

 

Step 45 – Rename it something meaningful

 

 

Step 46 – Then do an extrude.

 

Step 47 – Select the sketch of the piece to remove.

Step 48 – Change the extrude to do a remove

 

Step 49 – Adjust the direction so that it removes what we want.

Step 50 – Switch from Blind

Step 51 – to be Through all

Step 52 – Click the green check box to accept

Step 53 – To add this as a configuration, click on the Configure features button.

Step 54 – OnShape will enter the configuration mode.

Step 55 – Click on the extrude and notice the Unsuppressed check box that now appears.

Step 56 – Click on it and a yellow dotted box appears around the option and a new column appears in the configurations.  Click Done on the yellow box.

Step 57 – Notice that all of the variants have the Unsuppressed check box checked.

 

Step 58 –  But we only want to suppress it for the three variants so uncheck the others.

 

Step 59 – The Lip is removed, but time to check some other options.  Right click on the 8mm version and select “Switch to 8mm”

 

Step 60 – And the lip appears as expected.  It is worth checking a few other variants to make sure that they all behave correctly.

 

Step 61 – Now that the configurations have been done, click on the Configured part properties tab

 

Step 62 – We need to add the fields which change as the part changes.  First add the Name

 

Step 63 – That column appears in the list with all the values set to what was entered as the name for the part, next add the Description.

 

Step 64 – That is created and filled in with the Description (which was the URL entered for the part).  Click to add the Part number.  If there are other variances (such as Appearance or Material) then add them

 

Step 65 – Now that all the fields have been added, it is time to go through and fill them in.

 

 

Step 66 – Click on the name to select it.  Once nice short cut if the field is selected is to press the backspace key which causes OnShape to highlight the entire field.

 

Step 67 – Fill in the proper name (Name + SKU) for the part and hit return. OnShape will advance to the next row.  Press backspace to select that field, paste in the name, and keep repeating until the end of the column.

 

Step 68 – Repeat for the Description column.  If this is a part where they are all on the same page, then the Description could be kept to the default (assuming that is the URL that was entered for the part)

 

Step 69 – Repeat this process for the Part number entering the SKU.

 

Step 70 – Until it is all filled in.

 

Step 71 – To test, go back to the Configurations tab

 

Step 72 – And switch to a different variant

Step 73 – Click on properties for the part

Step 74 – And confirm that the correct values are there. Note that they yellow dotted line around the box indicates that it is automatically changed and filled in from the Configured part properties

Step 75 – Once you are satisfied with the configurability, select the Create version command.

 

 

Step 76 – Accept the version number and select Create.

Once you have the configurable template, it can be inserted into any assembly, but it is important to create the individual parts from the template so that a user can find them in the appropriate directory.  Instructions for doing that can be found in two parts

 

Creating the first configured part from a template part

https://drive.google.com/open?id=1oitQ62hTomvERxcR70H13NDVVi4qctw3lYd4ecytLbA

 

Creating multiple parts from the first configured part

https://drive.google.com/open?id=1IpKI1HMbqGvhxJVXs2pxwf_l9fSJnBIKDrFJqZv4MFc