Manufacture-ready 2D drawings

00:01

In this video, we're going to talk about how to create 2D drawings from Shapr3D parts. You start the process with an open Shapr3D project that has at least one solid body in it. It could have more than one, but it must have at least one. And then you continue by going to the File menu and create a new drawing. Alternately, you could use the SBI, the Selection Based Interface, and double click on a part to select it.

00:30

and use the create drawing selection in the menu. You could also select multiple bodies from the window and create a subassembly drawing or a drawing of multiple bodies. Name the new drawing. We'll just call this something creative, like new drawing. Select the sheet orientation, landscape or portrait. Select your sheet size and the default sheet scale.

00:58

You can tell Shapr3D to automatically include four views, or if this is off, you'll get the option to create the views individually. So with these settings, I'll just click Continue. The default view is the front view or the XZ plane, and we can project from there. I'll click on the plus to add the default view, and then I'll click on some additional views.

01:26

From here we have some additional options. One that you should pay close attention to is the third angle projection versus first angle. This is usually important when you have an ISO standard versus an ANSI standard. The title block can be simple as is shown in this drawing, or we could have a horizontal block, a vertical block.

01:49

or a block with a table. There are multiple options to choose from. I'm just going to go with the simple block, set your units. When you change these, all of the dimensions on the drawing will change. So you can do the drawing initially an inch and then switch to millimeter and all of the dimension values will update. Length format can be decimal or fraction. Angle format, again, decimal or fraction.

02:14

Length Precision, do you want two places, three places, four places? Angle Precision, same question. Decimal Separator, a comma is used in many countries, and so we've got the option to use a comma or a period, and that will go for all of the dimensions on the drawing. You can set your line widths for various types of lines on the drawing. Now you can move your drawing views around just by clicking on an edge and dragging them, and they will...

02:44

remain projected except for the isometric view. To further project views you can click on a view and select to add additional views. Some of these that see the back side of the piston are going to be better for me than the other views that were previously selected. When you're done projecting views click on the done button. You can delete views by double clicking on it and using the trash can. Clean up some of these views that we don't need.

03:14

move some of these around. You can also double-click on a view and use the arrows to move the views. When you double-click on a view you also get these badges that will allow you to change properties of the view such as the view scale or whether it's using hidden edges or not.

03:41

The section view can be created easily. Use the views section view option and you're being prompted what to do here. So I'm going to zoom in and click on a point that's on the center line and then click another point that represents the cut that I want to make and then click and drag to place the section view. Detail views can be made in a similar way.

04:11

So if I wanted to get a detailed view of the grooves around the piston, come over here, get the detailed view, drag a circle, click next, and then place the detailed view. Placing center lines is also easy. Go to the geometries option and a center mark is easy to place. You click at the point where you want the center mark to be shown.

04:37

and click Done to finish. You can also put in an actual center line. So in this case, I'll use a two line center line. There are several options. And I'll select this line and this line. This puts in the center line and I can extend both ends of the center line. And the center line could even go across multiple views.

05:05

if you had another projected view to the side. For example, down here, a center line could go through all three views. Dimensions are easy to create. There are several types of dimensions and you need to be aware of what you're trying to create at any given time. For example, if I want to create a diameter dimension, I'll select that option and go to an edge that shows the diameter I want to create and then place the dimension.

05:34

where I want it to go. Linear dimensions can be done in multiple ways. The most useful are the point to point and the point to line distance. If I had to pick one, I would use point to line. What this does is say up here in the scale view, I could go from this point to this line to place a dimension. And if I wanted to go from this point to this line

06:03

move these so they aren't on top of one another. You can use point to point dimensions in the following way. I'll select the point to point distance and select a point here and a point down here. The dimension is automatically placed here, which is not where I wanted it. I wanted it placed over here and to be a vertical dimension rather than horizontal. So you can click on the dimension, click on the badge,

06:31

and set this to a vertical dimension and then place it where you need it to go. So with the point to line dimensions, let's look at these again. The point to line distance, you use the line to establish the direction that the dimension will go. But with point to point, you can use a dimension option to set the direction that it will go. The other options with this were horizontal,

06:58

vertical and absolute just means you'll get an angled dimension from point to point. That's quite clever because that's sometimes exactly what you need. In this case, we need the vertical. Each dimension can also be annotated. If I click on the dimension, there's a badge that shows up. I can add prefix text, suffix text, and tolerances. So for example in suffix text, I might want to put the letters

07:28

typical groove width. There are some built-in symbols down here that you can also use and tolerances allow you several different options symmetrical, a deviation limits for high and low and a basic dimension. An angle dimension can also be created. Let's do one of these. There's several different angles. There's a three point angle, an arc angle, and the line to line angle. I'll demonstrate the line to line where I'll select

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this angled line and this reference line and that puts a dimension on. You can also create virtual sharps. That's under the geometries set of options and the intersection mark here will be between. We need an intersection between this line and that line. It's shown here by the point and also between this line and this line.

08:26

And now we can create a point to point distance between these two intersection marks.

08:35

Another available tool is the note and notes are easy. You can just click on wherever you want to place your note and then type in whatever you want the note to say. So we'll say grind surface flat, click in blank space to finish up. And then you can move the note around to suit your needs. We have the option also to show hidden lines on any particular view.

09:06

So let me select this view and the hidden lines option will show all the hidden lines for that view to add information to the title block. We can just come down here, double click on whatever needs to be changed and type in.

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the new information. And if you want to add an image to your drawing, you can use the Add Image button.

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Use the center mark to move it to the appropriate location, and use the corner buttons to resize it. This is a quick overview of Shapr3D's capabilities in creating 2D drawings. Other functionality should be intuitive and easy to find. Thanks for watching.