Skills Mapping

Dr L. Jabban - 11/12/2023

Skills ? :

Schedule:

Tuesday, Week 10 .

Creating an Assembly with CAD

Introduction

The aim of this lab session is to use pre-designed parts to create an assembly of the roller shown below. Assemblies are inventor files (.iam) that reference different parts and define the relationships between them to build an “assembled” component.

Once the assembly is done, an exploded view of the roller will be generated to illustrate the assembly sequence. This will be done using a presentation file. Presentation files (.ipn) are a file type in inventor used to [1]:

Create an exploded view of an assembly to use in a drawing file.
Create an animation which shows the step by step assembly order. The animation can contain view changes and the visibility state of components at each step in the assembly process. You can save the animation to a .wmv or .avi file format.

Downloading the parts

The parts used in the assembly can be downloaded from moodle using this link.

Creating the Assembly

Below are refresher videos if needed.

Please note that you can achieve similar results using the “joint” tool, as discussed in the lecture.

Creating an assembly file

To create a new assembly file, click on the arrow next to New and select Browse templates from the drop-down menu.

View of the drop-down menu to create a new assembly.

A new window will open with a range of templates from you to choose from. Select Standard (mm).iam to create an assembly, ensuring that the units are set to mm.

View of window to select the desired template for the new file. In this case, it is a Standard (mm).iam.

💾 Save your file somewhere you can access later. For example, your `H drive` or University `OneDrive`.

Adding components

Use the Place button to start the assembly by adding the base model.

Click anywhere on the working area to place the part.

Ensure you press esc when done to avoid placing multiple copies of the part.

Grounding the base

It is good practice to align the main part to the origin of the assembly file.
click on the + next to Origin folders to see the origin planes of the assembly part and base.

Assembly file showing the base and the expanded origin files to show the origin planes.

Click on Constrain in the top banner to apply the constraints.
Use the automatically selected Mate constraint type.
Click on the YZ plane within the assembly file.
Click on the YZ plane within the base file.
You will notice the base ‘snapping’ into position.
Click Apply.

Applying mate constraint to the YZ planes.

Repeat the same for the XZ planes, but clicking on the Flush option within Solutions to ensure that the base is placed facing upwards and to avoid conflicting constraints.

Applying flush constraint to the XZ planes.

Repeat for the XY plane, choosing the mate solution.

Adding and constraining the first bracket

Use Place to add the first bracket.
Note that you can use Free Move and Free Rotate to move the part to make it easier to apply the constraints.
Click on Constrain
Select the centerlines of the bracket and base, as shown below. This is done by hovering next to the hole until the centerline appears.
Note the change in the solution options.
Click Apply.

Applying mate constraint between the threading in the base and bracket.

Repeat the process with the second threading.
Try moving the bracket and you can notice that it will only go up and down relative to the base, keeping the threadings aligned.

Do not use the free move at this stage as that ignores the constrains.

Use the mate constrain to align the bottom face of the bracket to the top face of the base, as shown below.

Applying mate constraint between the bottom face of the bracket to the top face of the base.

Adding and constraining the bush

Use Place to add the bush.
Align the centres as shown in the screenshot below. Note that aligned is chosen within the Solutions.
Mate the end of the bush to the bracket as shown below. Make sure that you are selecting the currect surfaces.
Click apply.

Applying constraints between the bracket and bush.

Note that in this case, the assembly still has one degree of freedom as the bush can rotate along the centre.

Adding the roller and defining a joint

Use Place to add the roller.
Click on the joint tool and select the Rotational type to allow the roller to rotate around the bush.
Select the faces as shown below.
Click apply.

Creating a joint between the roller and bush.

Mirroring the bracket and bush

Given that the other side of the assembly is a mirror of what just assembled, the Mirror tool within the Pattern tab can be used.
Select the bracket and bush as the components.
click on Mirror plane.
Select the mirror plane to be the base’s YZ plane.

Note that you could use the assembly file’s plane in this scenario, but it is best practice to use the base.

Note that a pop-up window will show indicating that a new mirrored parts will be created. Click ok.

New mirrored files creating when using the mirror tool.

Adding and constraining the shaft

Using what you have learnt so far, constrain the shaft to result in the assembly shown below.
There are multiple ways to achieve this, feel free to use whichever you prefer.

Adding fasteners

The Content Centre within Autodesk Inventor allows for the addition of fasteners to be automated.

Within the Design tab, click on Bolted connection.
Choose Concentric from the Placement drop-down menu.
Choose the start plane, circular reference, and termination plane, as shown below.

Adding a bolted connection: Defining the start plane, circular reference, and termination plane.

Press Click to add a fastener.
A pop up window will appear with several options. You can filter them by selecting the ISO standard and Hex Head- Flanged Bolt category.

Select the ISO 4162 bolt. It should appear on the list of fasteners.
Note that a thicker line is present separating the components you can add on either sides of the surfaces.
Click on the top Click to add a fastener to add a washer.
Click on the bottom Click to add a fastener to add a second washer.

Note the length of the bolt adjusting as you add washers.

Click on the bottom Click to add a fastener to add a nut.
By the end of this step you should have something that looks like the screenshot below. If it does, click Apply.
Use mirror or pattern to add the rest of the bolts.

Adding Username

Do not forget to edit on of the visible parts to add an engraving with your username. You are able to edit parts while within the assembly environment.

Double click on the part you wish to edit to enter the isolate mode and use the 3D modelling ribbon used in the previous CAD lab.

Isolate mode to edit a part within the assembly environment.

Creating an Assembly Presentation

Below is a refresher video if needed.

Creating a presentation file

To create a new assembly file, click on the arrow next to New and select Presentation (.ipn) from the drop-down menu.

View of the drop-down menu to create a new presentation.

Placing the Assembly

Use the Insert Model button to add the assembly created earlier.

Press on Insert Model to add the assembly file .

Creating the exploded view

while pressing Control on your keyboard, select the 4 nuts added below the base.
Click on the Tweak Components button and select the arrow parallel to the direction of the nut.

Move the nut out by 75 mm.
Repeat with the washers, moving them by 35 mm
Proceed with moving components until you get the exploded view shown below

Exporting an illustration snapshot

To export a cleaner view of the assembly, you could change the visual style to technical illustration.

Within the view panel click on Visual Style and select Technical Illustration.

Move the assembly to get the view you want.
Click on New Snapshot View to capture the current view. It should get added to the panel on the right side.

To export it, click on Raster and adjust the settings as you wish. You may wish to select the transparent background option

The final result should look something like this:

You can also click on video to export the animation you created. If you click on the reverse option it will appear as if it is being assembled.

Application task

You can follow this link to download the parts for the application task. They are lego parts, enabling you to be creative in how you assemble them. However, below is a picture of a possible assembly should you wish to follow it.

Possible assembly of the application file.

References

[1] https://help.autodesk.com/view/INVNTOR/2023/ENU/?guid=GUID-94B779C0-6B2B-499A-A4F9-2E4BAB49712F

[2] Roller files designed by ROHAN GUPTA

[3] LEGO cad files designed by Hother - CPH Carpentry