>> This is part three of the lecture on SOLIDWORKS
and it will include the topic SOLIDWORKSSOLIDWORKS toolbox
and SOLIDWORKS drawings
which are also covered in lab number 23.
However, as you will see in the lab handout
for lab number 23 the student version
of SOLIDWORKS does not work.
It does not have the toolbox option
so you can skip that part of the lab.
So a toolbox is a collection of ready to use standard parts
such as bolts, screws, washers and so on.
It eliminates the need to create models
for the commonly standard parts and fasteners and they are easy
to drag and drop into your assembly or your drawing.
So under the toolbox browser, it contains a collection
of libraries here of the different toolboxes available.
And these libraries contain ready to use parts
and you can drag any part from the toolbox into your drawing
and you can snap it to the assembly and the placement
of a toolbox part is the same way
that you would place a part into your assembly.
So when the toolbox part snaps to the assembly,
they make relationships between the toolbox
and the other part is established.
When using washers, place them first and subsequent hardware
like screws and nuts automatically will mate
with this washer, we can change the properties
and customize this toolbox parts.
You can specify the properties that you are placing
and then you can also do that after the part has been placed.
And there is different ways of displaying them
with a simplified version, the cosmetic version
and the detailed schematic version
to show the threads of the fastener.
Toolbox supports international standards listed here.
The second part of this lecture is
on creating engineering drawings and which are assemblies
and detail drawings, as we called them previously.
So drawings communicate three things
about the object they represent, the shape using the views
to communicate the shape, the size and we use dimensions
to relay that information and other important information
which can be relayed to notes in the drawing.
Here is an example of an engineering drawing.
It is a detailed drawing of an assembly with dimensions
so it has views as well as this isometric here.
To create a new drawing in SOLIDWORKS you click on new
and click on drawing rather than a part or an assembly.
And here is an example of a drawing template,
each template is associated with a particular sheet size
that you are going to use
and each sheet you can edit the sheet or edit the sheet format.
This is two molds in drawing.
When you are editing a sheet, you are making changes
to your detailed drawing and this would be
where you would be spending 99 percent of your time
in creating your drawings.
You can add or modify views, add or modify dimensions
as well as text and notes.
On the other hand, to edit sheet format makes changes
to the title block and text headings.
You can make changes in the borders and these are things
that you add and in a lot of your drawings,
you can incorporate for instance company logo
and any other standard text that appears
in every drawing that you make.
We talked about title blocks before when we are doing the lab
on assemblies and detail drawings,
and here it shows how you can edit the title of block.
Under edit sheet format and when you go to the edit sheet mode,
this is where you will be doing most of your work
when you are making your drawings.
You can set the dimensioning standards by clicking on tools,
options, document properties,
you can click on drafting standard.
You can also change the setting for the text, text font by going
to tools, options, document properties and clicking
on annotations and then font.
Select the font that you want and then press ok.
Here is the general procedure
for creating a drawing in SOLIDWORKS.
You first open the part or assembly that you want
to create a detail drawing for.
Then you open a new drawing and design size,
then you add the views that you want to show
in your detail drawing, usually the 3 standard views, front,
top and right would be the most commonly used.
Then you insert the dimensions either automatically
or by importing them or manually
and then arrange those dimensions in the drawing.
Then add any additional information that you might need.
Here is an illustration
for showing the three standard views.
Click on standard three view, for instance, if you do this
on the part for Tutor One that we had from a previous lab,
it will automatically show three views.
Drawing number one, view number one is in the front,
number two is top, number three is the right side view.
You will select a view and click the,
to select the view you just click on the view boundary
and it is displayed in green.
And the relative locations
of the other views are, can be manipulated.
View one is the front as I said.
And the view too, can be moved vertically,
the top view can be moved vertically in the sheet
but it has to stay aligned with view one.
Same thing with view three it can move horizontally,
but it should stay vertically aligned with the front.
So you can drag it left or right.
Very important since for multi views including auxiliary views,
the headline should be shown.
So you need to set the setting hidden lines visible
for any view.
On the other hand, if you include isometric views
or sectional views in your detail drawing,
you generally do not show hidden lines for those.
So you will use the setting hidden lines removed.
Also very important, if you have a line of tangency
between two surfaces, so if two surfaces are tangent,
the transition from one surface to the other is smooth
and there should not be any lines separating them
so you need to select this option.
Tangent edge, tangent edges removed because that line,
the transition is smooth
so there is no actual edge separating the two
tangent surfaces.
So you can import dimensions into the drawing
and you can also add dimensions manually.
You can using smart dimension and there is associated
with these between import and dimensions and the size
or the actual dimension of the part.
So if I change the values in the import dimensions,
automatically the part size will change as well.
The same goes the other way, if I change something
in the part then for the important dimensions will
change accordingly.
On the other hand, for values that were manually inserted,
you cannot change them.
To import dimensions into the drawing,
just click on Model Items shown
and then click insert Model Items.
Click Import items to all views, meaning you are going
to add dimensions to all the views
where they should be added in the appropriate.
Click the options from marked for drawing and eliminate,
to click the checkbox.
So as we did in rules of dimensioning
in the previous lab, we try not to show duplicate dimensions
because they can confuse your audience, then click ok.
Once you have imported them, you can actually move the dimensions
because when it automatically generates the dimensions,
a lot of times they are not in an optimal position
so you can simply click on a particular dimension and drag
to change it location.
You can also delete dimensions if something is a duplicate
for instance, you select that particular dimension
and press the delete key.
You can click the arrows as shown here,
over here this is an issue usually
when there is not enough space between the width of the lines
to fit both the dimensions value itself and the arrows.
So here is an illustration, you have positioned the views,
arranged the dimensions by dragging them
in their appropriate locations.
So you want them to be aligned, you also want
to observe the rules of dimensioning that we have
and then set hidden lines.
Remove as well as a tangent edge, display and I talked
about this, changing a dimension will change the part,
the model itself and you will build it.
So if you want to play with it, try it, change the dimension
and you open the original part,
it reflects the new dimension that you set.
For multi sheet drawings, meaning containing more
than one sheet, here is an illustration the first drawing
to contain only for one part, Tutor one
and the second drawing could be for the assembly.
In the previous lab, we used Tutor one and Tutor two
to create an assembly.
So we can do multiple sheets, one for Tutor one only and one
for the assembly and we can do three standard views again,
as well as add an isometric view for the assembly.
Because for the assembly you want
to show how the different parts fit together.
Here is an illustration of the assembly, here is Tutor two
and here is Tutor one, here is the front top and right.
Then you can manipulate the positions
but they will stay aligned and the scale should be consistent.
The model here shows the part assembly
in a specific orientation.
You can use the standard views top, front right as well
as isometric view and you can also use any view orientation
that you want.
Say a trimetric for instance.
So you insert the model view, click model view.
Important, do not click directly on one of the parts
in this assembly, doing so will actually create a name view
for that specific part.
So here is more steps on doing this assembly
and as you can see we have added the isometric for the assembly.
Sometimes in addition to the three standard views
and isometric, you might want to show specialized views.
So a detail view, we already talked about that.
For so this is an illustration for a little view
of the switch plate, the section view,
so instead of just using the front top right
and isometric you might want a section,
you included in your drawing.
Here is an illustration here.