Lesson video

Hi there, everybody.

My name is Mr. Booth, and welcome to your Design and technology lesson for today.

It's wonderful that you could join me.

Today's lesson, Technical drawings in Fusion, you are gonna be creating technical drawings of the components that you have designed for manufacture.

This lesson is part of the Systems approach to design: Sustainable Future unit.

Today's outcome, I want you to be able to create a technical drawing using Fusion.

We have four keywords for you today.

First is orthographic.

This represents a 3D object in 2D, where views are projected from the object's faces.

We then have dimension, measurements added to drawings to define size.

Projected view, A 2D orthographic view projected from the base view.

And then finally, title block, a table containing information about a drawing, which we often use for manufacturing.

We have two learning cycles today.

The first is drawing fundamentals, and then the second one is about creating technical drawings in Fusion.

So let's get going.

Technical drawings are used to communicate information about a design.

They show dimensions, shapes, tolerances, and lots of other manufacturing details.

They also show the relationship between components and often how assemblies actually fit together.

Unlike sketches, they are precise and they are to scale.

Quick check for understanding.

True or false? Technical drawings do not need to be to scale.

Is that true? Is that false? Pause the video now, have a go at this, and come back to me when you've got your answer.

It is of course false, but why? Can you explain why? So pause the video again now.

Come back to me when you've got your answer.

Well, it is of course because they show dimensions, shapes, tolerances, and manufacturing details.

But unlike sketches, they are precise and to scale.

And when of course I mean sketches, I mean sketches that we do by hand, not the sketches that we do in Fusion, which are also precise and to scale.

Orthographic drawings show multiple views of the same design, usually from the front, top, and the side.

An isometric view can also be used to give a full representation of the design.

And here, we have a lovely example of a toy brick, and you can see we've got our 3D isometric view.

And from the isometric view, you can see we have projected our three other orthographic views.

We have one from the top, one from the side, and one from the front.

Technical drawings are used for manufacture and assembly of products by providing accurate information.

They are produced using standards such as the British Standard Institute or International Standard Organization.

And what this means is that designers, engineers, and manufacturers can use them no matter where they are in the world.

So if I design a product and I produce a technical drawing to an International Standard Organization drawing, I can send it over all the way to Japan and they will be able to manufacture it for me.

Here we have a technical drawing that has been produced in Fusion, and you might even recognize the part as the base component that we have been working on.

So here we have the border, we have a base view.

Now, quite confusingly, our base view is also our base, that component that we've been using.

We have a dimension, and there are a few of the dimensions on there that you can see.

We have a detailed view, which is a zoomed-in view of one of the projected views that we've got, and you can see this is of the micro:bit holder section.

We have a isometric view, the 3D view that we've got on that, and that's useful to have so you can see what it looks like in 3D.

We have a projected view which has been projected from the base view.

And then finally, we have the title block, which contains all the relevant information about the drawing.

Quick check for understanding.

I would like you to fill in the missing sections of this technical drawing.

Pause the video now, have a go at this, and come back to me when you've got your answers.

So what are those missing sections? Well, the top one is the base view, we then have the detailed view, and we also have the title block.

Well done.

So, like all the toolbars in Fusion, we need to be able to navigate them and know what they actually are, so let's have a look at the drawing toolbar.

So once you are in a drawing, your toolbar will change, and you'll have all these different features.

So the first one is create.

You can see we've got create in the top left and that's creating our views, our different views such as our projected views and also our detailed views.

We then have modify, do we need to move any of those or rotate any of those? We have geometry, so if we wanted to add things such as center lines, that's where we'd find them.

We then have dimensions, if we wanna add the measurements to our components.

We can add text, so if you want to tell any more information with leaders or anything like that.

We have symbols, so for example, if I wanted to add something about a surface finish, I could use a symbol from in there.

We have insert if we wanna insert any images.

And then of course we can create tables as well, which is very useful if you want to create a bill of materials.

And then we can of course export our drawing to something such as a PDF if we want to share it with anybody else.

We also have the title block and of course the canvas, and that is our drawing toolbar.

Now, for your first task, I would like you first of all to explain why designers use technical drawings.

And then what I'd like you to do is label all the sections of this technical drawing.

Pause the video now, have a go at this, and come back to me when you've got your answer.

So how did you get on? Well, let's have a look at some sample answers.

So first of all, explain why designers use technical drawings.

Technical drawings are used to communicate information about a design by showing dimensions, shapes, tolerances, and manufacturing details.

They show the relationship between components and how assemblies fit together.

Technical drawings are used for manufacture and assembly of products by providing accurate information.

Well done.

I then wanted you to label all the parts of this technical drawing.

So hopefully you got the border, the base view, the dimensions, the detailed view, the isometric view, the projected view, and you might have even got the other projected view at the top there, and also the title block.

Well done.

So we're now onto our second learning cycle, creating technical drawings in Fusion.

So to create a technical drawing in Fusion, the first thing we need to do is change the workspace we're in.

We're probably in the design workspace, and what we need to do is change that to the drawing workspace.

So if we click on the workspace where it says design, scroll down to drawing and then go across to From Design and click that.

A dialog box will then appear.

Now, we're gonna keep all the default settings apart from one.

We're gonna change the reference.

So the contents we're gonna change to Select, and then in our canvas, we're gonna select the base component.

Now, you can also select it in your browser by clicking on the component name in the browser.

So just make sure that we select base.

Once we've done that, we're gonna keep all the other default settings the same.

But it's quite interesting to look at what those default settings are.

So for example, the drawing is gonna be Create New.

The template is from scratch, so we're not including a template or anything like that.

We're using ISO standards, International Standard Organization.

Obviously we're using millimeters, and the size of our sheet is gonna be a three.

Click OK.

Quick check for understanding.

What standard is the default setting for Fusion drawings? Is it A, BSI, B, ISO, C, BIS, or D, IOS? Pause the video now, have a go at this, and come back to me when you've got your answer.

It is of course ISO.

Well done.

So let's carry on with creating our technical drawing.

So Fusion will now open the drawing workspace.

The first thing we need to do is place the base view on the canvas.

It'll be attached to our cursor.

We're gonna place it on the left-hand side, and actually probably a little bit higher to where I have signified it in that image there.

Once we've done that, what we need to do is change a few settings.

So first of all, in the drawing view dialog box, we're gonna change the Style to Visible Edges.

I don't want any invisible edges on that, I don't wanna be able to see through my components.

We're also gonna change the scale to 1:2.

So our design on our page is gonna be half the size of what the actual final prototype will be.

Once we've done that, we can click OK, and then just make sure we save the drawing.

Then in the Create toolbar, we're gonna click Projected view.

We've got our base view, so we're gonna use that as our base.

So we click on that and that becomes the parent, and our projected view is gonna be the child.

If we then hover our mouse below our base view, we'll get a preview of what it will look like, and you'll see it will look like we're looking down on top of our base component.

If we're happy with it, we click, click the green tick, and that will place our view.

Quick check for understanding.

What is the first view placed when creating a drawing? Is it A, base, B, bottom, C, projected, or D, top? Pause the video now, have a go at this, and come back to me when you've got your answer.

It is of course the base view, A.

Well done.

So continuing with creating our technical drawing, we need to repeat to add the third view on the right-hand side.

So once again, projected view, select the base as the parent, hover your cursor to the right, you'll see the view projected, drop it, and click the green tick.

We can also add an isometric view in exactly the same way, but rather than hovering our mouse directly to above or to the side or below our parent view, the base view, what we can do is do it at 45-degree angle and that will create an isometric view for us.

So make sure you've created all those views.

I also wanna create a detailed view.

So we have got a micro:bit holder, which actually is very small to see when we're at this scale.

So what I'm gonna do is I wanna do a zoomed-in version of that so I can have it to scale, so I can dimension that, so whoever is gonna manufacture this part can actually see what sizes I have used.

So from the Create toolbar, we're gonna click on Detailed View, which is that one there.

We're then gonna zoom in on the base.

And what we're gonna do is we're gonna select the base as the parent view once again.

And then where the micro:bit holder is, what I'm gonna do is I'm gonna click somewhere in the middle.

It'll snap to something in the middle.

And then that will create a circle.

And what we do is we make that circle bigger until we're happy that everything inside that circle is what we want to dimension, click, and then what that will do is create a detailed view.

Here, we can see the detailed view, and you can see it's underneath.

Now, what we can do is we can set the scale to 1:1, so it's gonna be exactly the same size as the final prototype.

Click OK, and then of course we can move it.

We can also move the text which reference the view as well if you need to.

So we're now gonna add some dimensions.

So from the Dimensions toolbar, click on Dimensions.

What we can then do is we can add dimensions in a number of ways.

I can do it between two points, between two lines, or even just click on a line if I wanna do a dimension from one side to the other.

Now, what I've done in this case is I've clicked on the top line and I clicked on the very bottom line and I created a dimension of 160.

I then dragged that dimension outside of my part and clicked to place it.

It's quite important to make sure that your dimensions are outside of the part where possible so it doesn't confuse the drawing.

You then need to obviously add all the relevant dimensions.

Try not to repeat dimensions.

There's no need to do that, and it's still actually a waste of data.

So what we want to do is use all the relevant dimensions that we think the person manufacturing this component would need.

We can also add radiuses and diameters in much the same way that we've done of the diameters.

So for example, on the micro:bit holders, you can see here I have dimensions, the outer circle and also the inner circle.

And you can see the differences between them.

And I've got my diameter symbol there as well.

It's exactly the same for radiuses.

So any of the rounds that I have or the fillets on the edge of my design, if I click on those with the Dimension tool, it will give me a radius of what they are.

And then finally, we need to fill in the title block.

Really easy to do, just double-click on it and it will open all the cells.

And what you need to do is fill in all the relevant information that you think you need in there.

Good ones to do are things like the title, who it's created by, date, approved by, and also which department you are part of.

And of course, we're all part of the design and technology department.

So we're now on to task B.

First of all, I want you to create a drawing of the base component.

I would then like you to add three projected views, add an isometric view, add all relevant dimensions that you need, and of course, fill in the title block.

Pause the video now, have a go at this task, and come back to me when you've completed it.

So how did you get on? Well, hopefully your drawing looks something like this with all the relevant information that you would need.

Well done with that task.

So we've now reached the end of today's lesson.

Let's have a quick summary.

In Fusion, you can create 2D technical drawings from a 3D model.

Orthographic and isometric views can be created that contain information for manufacturing.

Technical drawings contain projected views, dimensions, notes, and of course a title block.

Well done today.

You've been absolutely fantastic.

I look forward to seeing you all next time.

Goodbye.