Editing a Part which includes Screws in Onshape

Step 1 – Open the spreadsheet

Step 2 – Open document

Step 3 – Delete the assembly that is automatically created when you import the step file

Step 4 – Unpack the CAD Imports so that the STEP file is at the top level

Step 5 – And rename the step file

Step 6 – to be something simple like “Step” so that it doesn’t show up in the search

Step 7 – Update the document properties

Step 8 – With the name of the part and part number followed by a carriage return and the URL of the part

Step 9 – Select the screw(s) and delete them

Step 10 – You have to click on the green check to confirm the delete.

Step 11 – Select all of the planes

Step 12 – And hide them

Step 13 – Press Shift 7 to get to a nice isometric view

Step 14 – Click on the Transform function so that we can orient the part the same as it appears on the web page.

Step 15 – Change the Transform type to be Transform by mate connectors

Step 16 – Click on the part to transform

Step 17 – For the From mate connect, find a nice flat spot that represents either the top of the bottom

Step 18 – Then hide the part temporarily so that we can get to the origin

Step 19 – Click on the top of the origin connector

Step 20 – And unhide the part again

Step 21 – You will see the part reoriented.  If by chance you got the wrong spot on the origin, you can delete the connector and try again

Step 22 – Click on the reorient and flip buttons to get the part into the right orientation 

Step 23 – Click on the pencil next to the green check box to rename the transform

Step 24 – A name like Orient part works well

Step 25 –  Now that we don’t need the origin, go ahead and hide it.

Step 26 – Press shift 7 to get back to the isometric view

Step 27 – To insert the screw into the part, click on the Derived function

Step 28 – Select Other Documents

Step 29 – And find the ServoCity folder

Step 30 – then ServoCity > Hardware

Step 31 – then ServoCity > Hardware > Fasteners

Step 32 – ServoCity > Hardware > Fasteners > Screws & Bolts

Step 33 – ServoCity > Hardware > Fasteners > Screws & Bolts > Machine Screws

Step 34 – ServoCity > Hardware > Fasteners > Screws & Bolts > Machine Screws > Socket Head Machine Screws

Step 35 – Select the Sample 6-32 part

Step 36 – You should see the part studio to insert, but we need to know the screw size

Step 37 – Going to the page for the product, the specs usually give the screw length

Step 38 – Select the correct screw length in the configuration dropdown

Step 39 – And click on the Simple 6-32 screw part

Step 40 – Don’t forget to click on the pencil to rename the operation

Step 41 – A simple name like Screw will do here

Step 42 – To get the screw into position, click on the Transform function again

Step 43 – Change the Transform type to be Transform by mate connectors

Step 44 -Click on the Simple screw (many times it is hidden, so just click it in the parts list)

Step 45 –  To get to the mate on the screw, you may have to hide the part

Step 46 – Clock on the From Mate Connector and orient the model so you can see the bottom of the screw

Step 47 – Click on the bottom of the screw

Step 48 – Then show the part again

Step 49 – Rotate the part and find where the screw needs to go and click

Step 50 – You may have to flip the primary axis to get the screw into the right orientation

Step 51 – Click on the pencil next to the check to rename it

Step 52 – Call it something like Place Screw and click the green check

Step 53 – Select both parts

Step 54 – And find the boolean operation. Alternatively, you can use the Composite Parts Feature, at the top just to the left of the Sheet Metal tools(the far right section). It will create a composite part, which will behave just like a normal part, but will be in a “Composite Parts” folder rather than the “Parts” folder where parts usually show up.  

Step 55 – Sometimes the operation won’t work because the thread holes on the part are being difficult.  If that is the case, you can extrude the face of the thread down into the thread about .01” and retry the boolean operation.  Assuming that it works, click on the pencil to rename it. This step also applies to using the Composite Part Feature.

Step 56 – A name like Merge Parts works.

Step 57 – There should only be one part at this point in time, click on it and select properties. If you used the Composite Part Feature, right click on the composite part.

Step 58 – Enter the name and part number into the name field, the URL into the description and the part number into the Part number field.

What works well is to have copied the part name/number/URL fields from the spreadsheet and then paste it into the description.  Copy the part number into the part number field, then cut the Part name/number to paste into the name field.  It will also set up your cut/paste operation for later steps to rename the tab and document.

Step 59 – Scroll down and enter the vendor information and click save

Step 60 – Right click on the part to assign the material.

Step 61 – Using the information from the web page, pick an appropriate material.  Many parts are 6061 Aluminum for example. Click the green check to accept it.

Step 62 – Right click again to edit the appearance

Step 63 – Choose the appropriate color for the part.  Aluminum is #A5A5A5 by convention.

Step 64 -Rename the part tab

Step 65 – To the name of the part and the part number so that it shows up in searches.

Step 66 – Press Shift 7 to get a nice isometric view when you open the document again

Step 67 – And right click on the tab to select it as the document thumbnail

Step 68 – Also rename the document

Step 69 – To the same name as the tab with the part name and part number.

Step 70 – Click on the create version operation

Step 71 – Select the default name and click on Create.  At this point you should be complete!