Unit 4: Grade 11/12 Technological Design - Robotics - Driven Mechanisms - Gears, gearbox to wheel, drive train, and 1st function

Unit 4: Grade 11/12 Technological Design - Robotics - Driven Mechanisms

This unit will continue with robot sample design build and then your custom robot based on FIRST FRC robotics with a focus on mechanisms - gears, gearbox to wheel, drive train, and a robot function using SolidWorks.

Course Units and Descriptions

Use this table for an overview and navigate to each of the course unit pages.

Unit	Description
Review course outline for more details
1	Careers & Safety- Intro, computers, organization, and research career
2	Engineering Communication- Technical sketching, ortho-ISO, custom ortho, and robot design
3	Structure and Materials- Materials & measurement, joints, frame, and 3D model
4	Driven Mechanisms- Gears, gearbox to wheel, drive train, and 1st function
5	Functions and Integration- Body base, pneumatics, 2nd and 3rd function
6	Robot Assembly- Robot build, function supports, drawings and presenting
7	Marketing and Portfolio- Web authoring, portfolio and presentation

Unit Content Activity Quick Links, Click to Jump to Specific Activity!

Unit 4, Act. 1: Drive System Assembly

Situation:

With the frame of the sample and custom robot completed, the drive system can now be added. This process may involve making some more model parts and/or downloading and importing pre-made components, to start to build your drive system virtually in SolidWorks.

Problem/Challenge:

Create or download components needed for sample robot drive system, then create an assembly with the frame and drive system model components (sub-assemblies and parts). Using pre-made components, import them recognized or not into usable components in SolidWorks. Using the mating process, align and lock components to their correct locations to build your sample robot drive system. Folder organization for imported assemblies to be used for each wheel assembly, and sub-assemblies to be used for each front and rear drive systems. The main components you will be using can be found in your PMT pkg under the Material Cost Breakdown tab, an example table of what engineers use to keep track of detailed information on each of the components such as product name, descriptions, suppliers, part numbers,weight, web link, costs, etc. to later also include in drawings. Some of this list of components includes:

Single Speed, Double Reduction Gearbox
6" Omni Wheel
6" Traction Wheel 1.5" wide
VersaHub (1/2" Hex, Plastic)
Flanged Bearing
#25 Sprocket w/ Hub
Clamping Shaft Collar - 1/2" Hex ID
1/2" ThunderHex Stock
1/2" Acetal Spacer - 1/2" Hex

You will also create a set of drawing sheets (8) in a drawing file to include:

Drive system master assembly ortho/ISO, (overall DIM only)
Exploded drive master assembly system - balloons, and BOM,
Frame weldment ortho/ISO with 1 section and 3 detail views
Gearbox assembly ortho/ISO, (overall DIM only)
Omni assembly exploded - wheel, shaft, sprockets, hub, spacers with balloon and BOM,
Traction assembly exploded - wheel, shaft, sprockets, hub, spacers with balloon and BOM
Hex axle shaft weldment ortho/ISO (typical)
Hex axle spacer weldment ortho/ISO (typical)

Investigation/Ideas:

Design Build Options - Custom, Weldments, and Pre-made

To design and build your drive system, you will most likely need bushings or bearings to house the axles that will hold the wheels, drive transfer method components such as sprockets, and gear box. Axle could be sketched out, or in our case with the sample using the Thunder Hex shaft CAD part file, it can be downloaded and made into a weldment profile to use wherever it is needed. Anything with a pattern that is used multiple times at different lengths, a weldment should be used. Other parts such as wheels, gear boxes, sprockets, spacers, etc can be downloaded with STEP file, imported, and used to create the assembly of your build for the sample robot and/or your custom robot.

Recognizing imported STEP file is not necessary if you do not need to edit the part, thereby saving file space and complexity of your assembly. In some cases, recognizing errors may happen and you will have to use the imported step file as a solid unrecognized part (i.e. no editing of that part or assembly will be possible), unless you absolutely must have editing ability, then that component will have to made from scratch.

Importing STEP File (Hex Shaft Stock) into SolidWorks, and Creating a Weldment 2D Profile

STEP files are file formats that all CAD programs can read. There is a process to import them so they can be used in the program. This process can save you a lot time and effort. Why start from scratch or re-draw something that has already been drawn/made when you can just use a drawn design that is already made. The process below not only shows you how to import them, but also some best practices when making it into a 2D weldment profile.

Note, this does not always work if there is a technical problem reading the STEP file. When the tutorial was done below, there was no problem creating a 2D weldment profile, but interestingly with the upgrade of the operating system from Windows 7 to Windows 10, Solidworks now, will not recognize the features, therefore now it is not possible to do it with the same part file. Never the less, the process below can be applied to any part that can be recognized using SolidWorks FeatureWorks tool.

Importing a STEP File

Download the model STEP file and possible drawing specification file to a download folder, normally you will need to um-compress the file to view the STEP file. These files should be stored in a sub-folder with a descriptive name, such as shown, to later retrieve if necessary

Click yes on Import Diagnostics, then click on the green check mark, this is to check to see if file checks out

Automatically you will also get a window pop-up asking if you want to proceed wit feature recognition, click yes,

Then if necessary in the feature works tab, select appropriate options and finish with clicking on the green check mark to initiate feature recognition process

Once SolidWorks has recognized all the features and sketches, it will rebuild a new part file based original STEP file, which you can now use as a model part file to add to an assembly if needed

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Creating the Weldment 2D Profile from Imported Model File

First start by removing the Boss Extrude feature by right clicking in the tree on it and select delete

In our example with the hex shaft sketch on a offset plane 1, 9 inches from the front plane and ideally best practice would be to move the sketch back to the front plane

To move sketch from plane 1 to front plane, ensure the sketch you want to move is below the plane prior to selecting the sketch, then right click on it and select the Edit Sketch Plane icon

Click on the plus sign on the external features tree inside main window and select the front plane to move 2D sketch, then click on the green check mark

Fit your 2D sketch in the main window

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Add your File Properties such as the description, etc for the part you are working on

Right click on your sketch in the feature manager tree and select Edit Sketch

At this point you should see any dimensions and relations your sketch has

Right click on any part of the sketch and select "Fully Define Sketch" and

Ensure you have all the right options selected in the feature manager options panel, then click on the green check mark

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Additional relations and dimensions will be added along with dimensions

Clean-up dimensions, hide relations if necessary, and finish adding possible construction lines and references for future use

Add material type in the feature manager tree, by right clicking and selecting edit material type, the add specific material, in our case, aluminum 7075 t6

Once you have all information in 2D sketch done, exit sketch, select sketch in feature manager tree, then Save As, and

Save with appropriate file naming conventions with Library File Part selected as file type and locate your custom weldments folder and create a Hex folder for your new 2D weldment folder

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Importing, FeatureWorks, and Troubleshooting Resource Links

When you are using imported supplier CAD files, STEP files work pretty good and can usually be opened by SolidWorks and saved as a "dumb" SolidWorks part and/or assembly file. If you need control to edit that file it is possible to do some manipulation of the part file even if it is not recognized using the FeatureWorks tool. To get full control and edit the part fully, the imported CAD file will have to be recognized first using the FeatureWorks tool in SolidWorks. Be aware this does not always work and with our 2014 version of SolidWorks, as this version does not work well with Windows 10 in some cases, so some files will not work and result in an error and/or program crash. Several resource videos below go into detail on how you can manipulate imported CAD files.

Creating the Same Axle Weldment Profile From Scratch

For this same part that you require a weldment profile which the part can not be recognized in Solidworks and you were unsuccessful finding another part file that works, your next option is to use the original part dimensions/constraints to create a weldment profile from scratch. A lot of simple weldment profiles can be easily made from scratch and obviously should match standards that are used to manufacture, as your design needs to be based off of readily available standards that you can purchase and later build.

Create a new part using a sketch with two circles, one internal shaft hole, one for outside shaft rounds, with appropriate dimensions based off original Thunder Hex drawing, then using the hex sketch tool, create the hex and constrain to fully define and update material, in this case 7075-T6 (SN)

Fill in Summary information through file properties menu or properties icon on top, as shown in an example

In the same window next tab, fill in Custom information such as part number, finish, weight, material, etc (These two steps are good practices - newer versions do transfer this to the weldment and when creating drawings this information is handy when creating information tables)

Finish off your hex shaft using the Power Trim tool ensuring it is still fully defined, clean up dimensions if necessary

Shows constraints visuals turned off, ensure you have sketch selected in the feature tree, then Save As, a library file part in the appropriate weldment profiles folder, as previously learned when doing the robot frame last unit. Remember to name your part files using the previously reviewed file naming conventions.

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Creating a Structural Model Part (the hex axle shaft) From a 2D Weldment Profile

Now that you have prepared a 2D weldment profile form a STEP file or created the profile file from scratch above, here is a quick review to create a model from the same 2D weldment hex shaft profile.

To create the hex shaft weldment path, select the appropriate plane to sketch on, in this case the right side plane, and sketch your path and dimension the length to fully define it and if you want to centre it on origin a second dimension can resolve that

Shows the system options file locations for weldment profiles.

Select the Weldments tab, then Structural Member, then select your weldment initial standards folder, then select the type folder, and then for the size folder, select your previously named 2D weldment sketch file. It is a good idea to angle the 2D weldment path in an isometric angle for future viewing

With your 2D weldment sketch file selected, right click on the 2D path line for weldment profile to follow, a yellow preview will show. In some cases you may have to change the alignment, angle, or profile mirror to get it just right, in our case the centre reference is good, so click on the green check mark

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SolidWorks will show a finished view of 2D weldment profile following 2D path. In newer versions, when you use 2D weldment profiles, it gives you the choice to also transfer the material type over, but for 2014 version you will have to add it again here manually

Check or update your file properties summary and custom entries to ensure it has what is needed such as description, material, etc. This information is usually used later in tables - to identify characteristics of that part in particular related to other model parts and drawing auto-fill fields in the information block

Use the Save As to save the weldment part file with appropriate file naming convention, and save to your robot root directory. As this is a part of your drive system, you could make and put it in a sub folder called drive system, or a better/recommended option is to just add the category drv to your file name such as td3-1_j-doe_drv_axel_P_HEX_AL_0.5x3.SLDPRT, so that later when you add more related drv models and assembly files, they are organized and will be easily found

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A little About Fasteners

It is important to keep your fasteners for your project as few as possible in terms of types and sizes. Using a few common sizes on your bot will save a lot of frustration when doing repairs, finding tools, and keeping everything simple. For example, use a common rivet size that will work all over the robot. Using similar thickness sizing with rivets means you can make your rivet with a depth to cover common 1/8" or 0.125" sizing. This would mean you would need to make your depth 1/4" or 0.25". You also have the option to download common fasteners that you use from CAD suppliers online. Solidworks has an add-on called toolkit, which has a set of standard fasteners that you can also use.

Generally you put your fasteners on as the last thing as to not over complicate. It is simple enough to match hole from one object to another by using the tool "Convert Entities", and ensure that your mates are all good.

Create/Construct:

Sample Robot Drive System

The robot drive system requires you to build both of your wheels with the track wheel being more complex. Most of the parts are manufactured, so you will practice working with imported pre-made parts- not recognized and some that are needed to be recognized, because you need to modify for your own design, i.e. edit them for your own use/design.

For your convenience, you should find all of the components already downloaded into the pick-up folder under Resource Library\CAD\MF CAD Drive Sys Dwnlds so you don't have to search for them online. Also included in each folder are PDF support papers on each of the components detailing their specs and any other pertinent information.

Remember folder/file use and naming convention, name features in feature tree, add the summary information, properties, and material for each of your custom parts made. Manufactured parts used, should be in the school networked share CAD folder library. Ensure you have your edrawing file: mf_drv-base_A_35x27.easm open for reference. Below are the basic steps to complete the robot drive system.

Steps:

Be aware that in the PMT Pkg the material cost sheet has links for all of the parts, for example: to download the axle CAD STEP file, which you would normally use to create your own weldment profile for multiple weldment parts of the same shape, but in this case, will not recognize while other parts will work. Remember to keep-in-mind the sample folder structure picture, folder/file use and naming conventions section for organizing your robot CAD files before you start on the next step - i.e. keep this as a high priority throughout the project

Because the STEP axle file will not be recognized since Windows 7 update to Windows 10, (ideal time to take a recognized part file to create a weldment profile), you will need to create a 2D weldment profile from scratch, then create a 3" drive shaft weldment part for the sample robot. Create the shaft spacer weldment profile- if it will not recognize with FeatureWorks, to use the profile, then you will have to also make from scratch - see eDrawing for spacer size lengths required for drive system

Get or download the flanged bearing and import the STEP file with no part recognition as the bearing does not need to be edited or modified (plus an error will occur if you try to recognize it) and save as a SolidWorks part file for placement on robot frame assembly in step 5

Create a drive system assembly file using your frame as the initial component and locking the frame model origin to the assembly origin (fixed). This is done by selecting it as your first part of your master assembly and click the green check mark without placing (clicking) in model/assembly space - this way the frame will by default automatically align/constrain to the origin. The other option is to manually do it by using mates to lock all planes of the assembly space to the component brought into the assembly using the the coincident mate tool

Start by placing your bearings into your front, middle, and rear shaft hole locations with the bearing flanges facing to the inside of the frame (remember, have the eDrawings sample frame open, for precise view of part locations, placement, and position)

Frame

Omni

Track

Omni

Track

Make sure you are building just the left or right side only, as you will later mirror the wheel model parts in the assembly to the other side using the front plane

Start on Omni wheel assembly, by first opening the STEP file wheel assembly to save as an assembly to a sub folder, to keep parts organized and separate because this is a pre-made component with lots of parts, and better to keep all of those imported parts in a group. Also get the Versa Hub, and 25 tooth sprocket with hub will need to be imported to part files. Remember, FeatureWorks recognition is only needed if you need to edit that "part" specifically, you do not need to edit these parts as you are going to use as a "dumb" SolidWorks part file. You will also need the hex shaft and spacer weldments you made earlier

Create a new Omni wheel drive sub-assembly using the axle as the fixed initial part, with appropriate mates to place and mate omni wheel sub assembly, hubs, spacer, 25 sprocket. Once all together you can take your Omni wheel drive sub-assembly and mate to your drive frame assembly - mating to bearings inside your robot frame (remember, just do one side, you will mirror later)

Get the traction treaded wheel STEP file to save as an assembly. You will need to create the right wheel width by removing a tread and wheel frame ring after getting the STEP file saved as an assembly in its own folder. As this assembly will not have mates, suggest you "fix" all parts before editing assembly and just float those parts you need to mate for appropriate re-fit (not the norm, to have all fixed) then edit Torx screws, and hex wheel spacers or bring in new ones to position and mate as needed to end up with a completed 1.5" width traction wheel

Create a new traction wheel drive sub-assembly with your hex axle as your fixed part and adding your updated 1.5" traction wheel assembly, the Versa Hubs, 25 tooth sprocket with hub, and hex shaft spacers, and then bring into your main frame drive assembly

Download/get the gearbox STEP file and save to an SolidWorks assembly, the 16 tooth sprocket, and shaft clamps for adding to the drive frame assembly. It is important to align/constrain the gears from gear box shaft to the front and back gears for chain alignment (This will be checked to see if they are lined up and constrained to each other!). Before you mirror any sub-assembly components - front/rear wheel systems and gearbox, ensure there are absolutely no problems and all mating is done correctly, as mirroring it will compound problems/errors further

Use the Mirror tool to mirror the front wheel sub-assembly, rear wheel sub-assembly and gearbox sub-assembly to the other side of frame using the front plane to finish your drive assembly. You will most likely have to work with the options and configuration of the mirror feature tool to get them mirrored properly

Drive System Assembly

Re-open each drive wheel sub-assembly, and create an exploded views in the configuration tab panel, spacing out each component appropriately for later use in showing in your drawings

Now you are ready to create a drawing set as required in the Problem section above. Use the provided template and remember for the drawing information block fields to fill, you need to have those custom properties and the summary information correctly filled in in the related parts/assemblies

Create exported JPG's and eDrawing files for your work completed, but it is not necessary for supplier CAD work - just work from scratch and work created from supplier CAD files

If you are stuck on something remember you can review related links in the Investigation section above and the previous unit, collaborate with your partners, and when done, use a peer to check your work before handing in, in hopes to find fixes and updates to improve your mark for this project.

Custom Robot Drive System

Time permitted, using the above sample process, apply it to your custom robot, by adding your drive system to your frame, creating your assembly, exploded views, then creating a set of drawing sheets and an updated cost material sheet

Evaluation:

You are responsible to hand in your sub-assembly drive system as a separate folder for evaluation, with the master assembly (that which holds all the sub assemblies together- drive system, elevator, gripper intake, etc) will be looked at in Unit 6.

Make sure your folders, files, organization, and naming conventions are saved correctly, files open up to appropriate views (for example model part and/or assembly - full screen with best ISO view), all CAD files working (double check parent files if you have changed file/folder names), and include full page JPG images and eDrawings of all CAD work completed. Ensure you have completed the SolidWorks Self/Peer Checklist sheet when you hand in your digital CAD files. This self/peer evaluation sheet (worth 10% of project mark) and is there to help you hand in the best product showing your process build, get written feedback on your completed work, and a mark breakdown.

Evaluation Breakdown Component Descriptions	Marks
Always double check that you have completed all components for full marks.
Axle - finished axle model part from 2D weldment profile process	15
Drive System - Sub & master assemblies,, exploded wheel views	50