FROM 3D TO 2D DRAWING BASICS

FROM 3D TO 2D

With any CAD system you can create the views that you need, to make a 2D drawing of the 3D Parts/Assembly that you created.   You could start by using the command “Open” a 3D CAD file

  1. File – New – Drawing Stencil – Create

The next step is to create the views needed for all the dimensions.   You would usually use 2 or 3 2D views and one 3D view for the material call out (explained more)

To create the views:

-Click on BASE (upper left corner)    CAD system will automatically create the base 2D view.

-Drag mouse up then left click for the 2nd view and to the right of the base for the 3rd view

-Drag mouse in the right upper corner then left click for the 3D view – then click OK

When the base view is created you can rotate it as you wish using the arrows from the right. On the left window you can modify the scale and the Style. You can always come back to this window to make changes.

On the left menu you will find Drawing Resources and the type of page being used which will always be A3 landscape (ledger) which you can then change to the type of page suitable for the drawing.

Next it is important to change the page size:

-Right click on A3 – delete

-Right click on 1 – edit sheet

The other page type that we constantly use is A4 Portrait and A2 Landscape for Assembly Drawings. After changing the page size you have to replace the border. To do that go to:

-Drawing Resource – Borders

Choose the border corresponding to the page size and double

Click on it.

BORDER INFORMATION

On the right down corner of the border there is a legend that needs to be filled with information about the part and the drawing.

You fill the empty spaces by using FILE – Properties – Project

  • Stock number = quantity
  • Description = scale
  • Revision number = part number
  • Project = project number
  • Cost center = material

DIMENSIONS

You need to dimension the part so that it will be easy for the people who fabricate it to read all the dimensions.

As a general rule a part will have:

  • Overall dimensions
  • Holes positions (if the parts has any)
  • Holes types and diameters
  • Chamfers and radiuses dimensions
  • Marked machined surfaces
  • Any other dimensions needed

We usually use two types of dimensions:

  • Regular Dimension

– Used for overall dimensions and any other dimensions

  • Ordinate Set dimension

-used for marking the holes positions and machined surfaces.

OVERALL DIMENSIONS

Overall dimensions are measured from the most left point to the most right point of the part and from the most upper point to the lowest point of the part.

Use the Dimension button from the upper toolbar

 

Examples

HOLES POSITIONS

If the part has holes you make their centers visible and mark their X and Y positions using one of the edges/faces of the part as reference. We usually use either machined faces or the furthest edge/face from the holes as reference.  To make the centers of the holes visible:

– Right click on the view – Click on Automated Centerlines

Using the Ordinate Set button from the upper toolbar you mark the holes X and Y position.

Click on Ordinate set – click on the reference edge – click on all the centers of the holes – right click – continue – drag the dimensions to the left/right or up/down – right click – create.

It is recommended to use the same zero position for the Y direction and the X direction, making it easier this way for the people who make the part.

TYPES OF HOLES AND DIAMETERS

Parts usually have the following types of holes:

  • Through holes
  • Thread holes
  • Dowel holes
  • Counter bored holes

Each type of hole has a standard

Symbol.

THROUGH HOLES 

A through hole, also thru-hole or clearance hole, refers to a hole that is reamed, drilled, milled etc., completely through the material of an object. In other words, a through hole is a hole that goes all the way through something.  On the drawings they are going to be represented by a regular circle symbol.

Use Dimension button from upper toolbar to mark its diameter.

Click on the edge of the circle – drag – click –OK.

If you have more than one of the same dimension put the quantity in front of the diameter in the window that pops up after you click.

THREAD HOLES

Holes that have threads in order to fit a particular screw size. They can go all the way through the part or reamed, drilled, or milled to a specified depth without breaking through to the other side of the work piece, also known as TAP HOLES.

On the drawings they are going to be represented by a circle within a circle symbol (the circles will be very close to each other unlike the counter bored holes where you can see a significant distance between them)

Same dimensioning step as thru holes!

For thread holes instead of Ø you use M8, M5, M6 etc. To do that, after you drag and click check Hide Dimension Value and manually input M8,M6,M5 etc.

DOWEL HOLES

On the drawings they are going to be represented by a simple circle symbol and you have to insert a dowel hole symbol. You can find the dowel hole symbol in the left toolbar under Drawing Resources – Sketch Symbols – Dowel Hole

Double click on the size you need and place it on all the dowel holes. You need to add tolerance for the dowel holes diameter and positions.

Dowel holes need the machining symbol added like in the drawing above.  Go to Surface button (upper toolbar) – click-drag-click on dowel hole dimension arrow.  Select second Surface type – A” =25Z

 

COUNTER BORED HOLES

A counter bore (symbol: ⌴) is a cylindrical flat-bottomed hole that enlarges another coaxial hole, or the tool used to create that feature.

On the drawings they are going to be represented by a circle within a circle symbol (the circles will be far apart from each other unlike the thread holes where the distance between them is very small)

Same dimensioning step as through holes!

Manually input the following information:

-THRU

-|___| (counter bore symbol)

-outer hole diameter

-depth symbol

-depth value

CHAMFERS AND MACHINED SURFACES

Chamfers

A chamfer is a transitional edge between two faces of an object. It can also be known as a bevel but connotes more often cutting and is more often 45° with respect to the two adjoining faces.

For dimensioning chamfers we use the Chamfer dimension button from the upper toolbar.

Machined surfaces

For machined surfaces we use the Ordinate Set dimension button from upper toolbar. Add the machining symbol added like in the drawing on the right Go to Surface button (upper toolbar) – click-drag-click on dimension arrow.  Select second Surface type – A” =25Z

CALLOUT

Is a short string of text connected by a line, arrow, or similar graphic to a feature of an illustration or technical drawing, and giving information about that feature. In this case it represents the overall dimensions of the part: thickness x width x length

For Callout we use the Leader Text button from The upper toolbar. Click on the part you want to Callout – drag and then manually input thickness X width x length

The thickness will almost always be expressed in inches. The width is usually also in inches. The length is usually in mm.

ASSEMBLY DRAWINGS

FROM 3D TO 2D

For the Assembly drawing you will follow the same steps as for the parts drawings. Assembly drawings need 3 2D views and one or two 3D views so you can balloon all the parts that make the assembly.

Assembly drawings usually consist of:

  • Three 2D views
  • One or two 3D views
  • Overall dimensions
  • Balloons from all the parts that make the assembly
  • Balloons from all the purchased parts

Before ballooning all the parts import the parts list so you can rename the parts according to the drawing name. To do that go to Parts List button from the upper toolbar – select the file corresponding to the assembly – hit OK- drag the list outside of the drawing area.

To modify the parts list double click on it and rename the Parts so that the part number matches the drawing number All purchased parts will be numbered using 601, 602, 603 as an example and so on.

To balloon the parts go to Balloon button on the upper toolbar – click the part that you want to balloon – drag – double click to release.

BORDER INFORMATION

On the right down corner of the border there is a legend that needs to be filled with information about the unit and the drawing.

You fill the all empty spaces  (except project name) by using command FILE – Properties  – Project

  • Stock number = quantity
  • Description = scale
  • Revision number = unit number
  • Project = project number

The date & designer field  and drawing name is often filled automatically when you create the drawing.  If possible input the project name you go to File-Properties-Summary.

UNIT REQUIREMENTS FOR MANUFACTURING STANDARD THICKNESS

Parts modeled with manufacturing thickness considerations require standard sizing as shown in the chart below for which many components are sourced together.

“FROM 3D TO 2D DRAWING BASICS”                                2023 Copyrighted by illustrative designs, LLC

 

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