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  2D Sketch / 3D Part  -> Assembly and Simulation  ->  2D Detailed Drawing    

INTRODUCTION: Parametric 3D CAD Drawing using T-FLEX; for a brief video click HERE. Initial principles:

• Designs are saved to ".grb" files; each file can save multiple "Window" spaces linked to a single model.
• Uses a parametric feature-based simultaneous solver; 3D shapes are linked to "parent" sketches, which in turn can be linked to spreadsheet files, etc.
• Some concepts (Sketches, File Windows, Model Tree, Construction Lines, etc) may seem similar to Pro/ENGINEER
• Most commands can be applied to create/modify either 3D closed solid or open surface -type shapes
• Most commands have Options (see Automenu) and Parameters (See Properties Window)
• Often there is often more than one way to perform most tasks in T-FLEX CAD
• T-FLEX .grb files can be externally referenced into other .grb files as "fragments" (either in 2D or 3D - more about this feature in our detailed drawing and part assembly tutorial pages).

T-FLEX User Interface:
1. Main ("Top") Menu
2. System Menu, Palette Windows (below) & "Mode" icon 
3. Command Toolbar for current "Mode"
4. Selection Filter mode buttons
5. File (i.e. "NONAME1") and Window ("NONAME1:1") tabs
6. Context Menu - a right-click context command list
7. Interface menu (turn on/off toolbars, palettes, etc)
8. Status bar
9. Location for Automenu (in-command options)

Mouse Buttons:
LEFT: Select (or 3D dynamic rotation when clicked in empty space)
MIDDLE: Pan real time (up-down/left right)
SCROLL: Dynamic zoom, "in" and "out"; "Scroll pointer" through overlapping elements - requires mouse hover & brief wait - see here right ->
RIGHT: Open Context ("pop-up") command menus; cancel command

Tooltips:
A description appears for command icons as the mouse hovers over them.

The T-FLEX interface uses numerous flyouts, context boxes and cascading pop-up menus - which can be disorienting for some at first. But as T-FLEX becomes more familiar to the user, these can be used to great advantage.
Accept new shapes or changes from any tool or command by clicking Finish or by pressing the ENTER key.
Stop using any command or tool by clicking Cancel to return to the previous toolbar menu. You can also press ESCAPE or right-mouse-click to stop using a tool/command.

3D design in T-FLEX starts with a planar (2D) sketch. Note a part sketch is not a 2D detail drawing (discussed HERE).
1. To start a new 3D part file, select "File -> New 3D Model" from the main menu. This will create a new file "NONAME1" and open a new 3D workspace Window.

2. Right mouse-click on any 3D plane; for this example the Front plane has been chosen..

3. A Context Box will briefly appear above the plane

4. From the Context Box select "Draw On Workplane" --> 3D Window view will be automatically re-oriented to draw "flat" on the selected plane (normal view). 

5. Mode change : from Workplane to 2D. The command toolbar should change, now showing a set of icons used for creating 2D sketches.

Construction geometry serves as a mathematical reference "skeleton" for complex sketches and is offered in several CAD systems. The concept is similar to a table draftsman first drawing light 6H measurement lines to be connected later using stronger 2H or HB pencil strokes. T-FLEX constructions establish visible references, measurements and relationships for constraining the final sketch. They also explicitly capture design intent. Part sketches may be quickly created without construction geometry - just using Graphic lines - but constructions add more functionality to the sketch. To create a construction based sketch for a 3D model:
 
6. From the command toolbar along the top, select the construction "Line"   and this tool's Automenu (shown left) should now appear within the previously empty central column of our T-FLEX interface(9). NOTE: Always check a command's Automenu carefully to see what options are offered.

Quick example - creating "construction lines" in a T-FLEX CAD sketch:

2D part profiles can be created from our construction geometry using the Graphics tool (inkwell pen) or the Hatch tool. For this example we want to create a closed square/rectangular sketch.

Using the Graphics tool

The Graphics tool is used for "darkening" a final profile over top of existing construction geometry. Graphics can toggle between two modes of operation from the Automenu: Free mode "on" or "off" . With free mode "off", Graphics will "snap" to the nearest implicit point of two intersecting construction entities upon each left mouse click selection. This allows the designer to quickly close off a final outline. Right click again to finish command.

Our final rectangular outline should be closed.

NOTE: If you hover your cursor near any of your new construction lines, they highlight green and if you hover over any of their intersections the implicit points highlight with a blue box.

Sketch Dimensioning

The Dimension tool (also called "parameterization") creates measurement constraints. It is found in the top Command toolbar (again, with the 2D "Mode" still selected). It allows us to create dimensions in our sketch to edit and change them by entering new measurements, etc.

Click the "Dimension" tool . Select one side of our sketch profile. It should highlight red. Now select the corresponding parallel side and you should notice a dimension appear between the two sides with a value of the distance. Then select a location for placing the dimension text. Cancel this tool when finished.
 
To edit and make changes to your dimensions simply select the new dimension text and a box should open up for editing the distance value . Click "Finish" or press ENTER to apply the changed value. Sketch geometry will be automatically redrawn with the new distance value. (or click "Cancel" or press ESCAPE to discard the change)
 
Once you have finished right click somewhere in empty workspace to open the context menu. Click "Finish" . This will save the sketch change our view back to 3D view with a new profile on selected plane corresponding to the final 2D sketch.

3D Part Design "pulls" 2D profiles into 3D shapes:

1. Select (left click) our profile (rectangle sketch) entity from the workspace. A finished sketch appears as a green profile by default. Alternatively, our profile can also be directly selected along the 3D Model Tree, which is usually the far left palette tab.
 
2. A Context Box* should appear above the mouse. Select the "Create Extrusion" tool.
*NOTE in 3D design the Context Box is an abbreviated version of the full Context Menu (discussed above). The Context Box is opened with a left-click + entity selection to start a new command. The current Context Menu is opened with a right-click at any time during design work.

Upon clicking the "Create Extrusion" tool, a preview of the resulting 3D shape using current default distance is displayed. The distance values appear in temporary yellow dimension tags on the part. These tags can be dragged by selecting and moving them, or edited by clicking on their value and changing it to a new number. While the original sketch remains green in colour, our 3D preview shape will have white edges by default setting.

There are several initial ways to specify the length of extrusion in T-FLEX CAD. The dimension tags may be edited directly by typing the value. Alternatively, when the mouse hovers over an edge belonging to the preview shape, it may suddenly become an "Offset" pointer which allows the user to "drag" either side of the extrusion to its desired offset value. It may take some practice to start or use the use the offset cursor.

3. For this example assign a 100 distance to one side and a 64 distance to the other as shown here left.

4. Click on the Finish icon (green tick) in the Automenu to save this new 3D box part.

5. To edit this shape again afterwards you may notice the 3D Model tab docked on the upper left hand side. Click 3D Model tab > Body_0 > Extrusion_0 and Right click > edit. Make any necessary changes to the extrusion if necessary and click Finish in Automenu to save changes. You can also go back and edit the dimensions of the shape by clicking 3D Model tab > Body_0 > Extrusion_0 >3D Profile_0> Front and Right click > Edit. Click Finish in Automenu to save changes.

Sketch on 3D Face - Draw an Ellipse

2. Click "Draw on Workplane" from the context box. If you wait too long, the context box disappears and you will need to either: a) right-click to open the full Context Menu or b) unselect and re-select the face again.
 
3. T-FLEX automatically rotates the view for easy sketching. Make sure you are in "2D" command Mode . We are now going to draw an ellipse.
 
4. We first start with two points, or "Nodes". Select the "Node" tool from the Command toolbar. The Node Automenu should appear. Turn on "Free mode" (top icon in Automenu). "Free mode" allows us to place the nodes anywhere on the 2D sketch.

5. Select two diagonal locations well "within" the visual surface area of our 3D box. A tiny red box represents each Node that was created, as shown right. Right-click once to exit the Node tool.

6. By default, construction lines appear "white" if colour is set to black. We need to change the system colour to something else (red) since our 3D box creates a "white background shape" in this 2D sketch. Select a new colour from the colour menu in the System toolbar.
 
7. Select the "Ellipse" tool from the Command toolbar. Curve creation offers two modes in its Automenu: specify edges or specify centres . Click on edge mode and select our two Nodes. A temporary ellipse will now "rubber-band" until we click to locate a final point to define the mathematical eccentricity of our ellipse (dictated by our semi-axis length). Result is a dashed construction ellipse. Finally click "Cancel" to exit this tool.
 
8. Select the "Hatch" tool from the Command toolbar. Like Graphic lines mentioned earlier, the Hatch tool "marks" what region of construction geometry gets passed to 3D space as a final profile. NOTE associative hatches are created by defining temporary, closed contours (i.e. "regions") from construction entities. Complex "Contour Autodetect" requires Graphic outlines to be already defined (see above). However, simple linear and arc contours can also be defined directly from construction entities themselves...

9. From the Hatch Automenu, select "Manual Contour Input" mode. This will trigger several direct construction selection options in this Automenu. From the Automenu click "Create Ellipse Contour" and select our ellipse sketch. The ellipse should turn blue with an arrow indicating the contour's direction, shown here right. Click "Finish" . The region contained by our ellipse should now be hatched by a pattern of lines. Right click to exit this tool. Right click again and click "Finish" from the Context menu to return to 3D space.

3D Boolean Feature - Creating a Hole

A Boolean feature modifies an existing "target" body(s) with geometry applied from new "tool" bodies . 3D Bodies are combined into complex models by either adding to (like a lump), subtracting from (like a hole), or intersecting with existing (target) geometry. The boolean mode is changed via the Automenu. This usually appears as a small fly-out icon at the bottom of any command's Automenu (requires holding a left-mouse-click momentarily down on icon to open, as shown here right).

2. From bottom of the "Extrude" Automenu click and hold the mouse button down briefly on the Boolean mode to open the Boolean flyout. Change the Boolean mode to "Subtraction" . We are creating a hole.

3. Most T-FLEX commands also have additional "parameters" which can greatly adjust a command's result. These parameters are changed via the "Properties Window" tab, which is normally docked upper left among several other palettes and surfaces when a command offers additional parameters. In the "General Parameters" section, change the "Forward" parameter from "Automatically" to "Through All", as shown here - right.
 
4. Click Finish . The 3D box now has an elliptical hole.

Editing Parametric CAD Features in T-FLEX

To edit go to the 3D Model tab on the your left. 3D model > 3D construction > 3D profiles > 3d Profile 1 > Workplane _3. Right click and select Edit geometry. This will take you back to the shape you had drawn before and allow you to change its size or even change the shape entirely. Once you have finished simply right click and select Finish . Your changes will be automatically updated in the 3D model.

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