2D Sketch / 3D Part
-> Assembly and Simulation
2D Detailed Drawing
Parametric 3D CAD Drawing using T-FLEX; for a brief
- Designs are saved to ".grb" files; each
file can save multiple "Window" spaces
linked to a single model.
- Uses a
simultaneous solver; 3D shapes are linked to
"parent" sketches, which in turn can be
spreadsheet files, etc.
- Some concepts (Sketches, File Windows, Model Tree,
Construction Lines, etc) may seem similar to
- Most commands can be applied to create/modify
either 3D closed solid or open surface
- 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 .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:
Palette Windows (below) & "Mode" icon
for current "Mode"
Filter mode buttons
"NONAME1") and Window ("NONAME1:1") tabs
- a right-click context command list
menu (turn on/off toolbars, palettes, etc)
Location for Automenu
(or 3D dynamic rotation when clicked in empty space)
real time (up-down/left right)
, "in" and "out";
"Scroll pointer" through overlapping elements
- requires mouse hover & brief wait - see here right
RIGHT: Open Context
("pop-up") command menus; cancel commandTooltips:
A description appears for command icons as the mouse hovers over
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
new shapes or
changes from any tool or command by clicking Finish
or by pressing the ENTER
using any command or tool by clicking Cancel
to return to the previous toolbar menu. You can also
to stop using a
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.
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.
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
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:
7. Click "Select 2 crossing
lines and node"
from our Automenu. Note the mouse pointer
now "carries" two crossing dashed lines.
This tool places two infinite perpendicular
construction lines at any location(s) selected in a
8. While "in" the "Crossing Lines" tool, select 2 diagonally
opposing locations somewhere in the design space.
Our result should look something like a dashed tic-tac-toe grid (as shown right):
9. Click cancel
or right-click to finish using the "crossing lines"
2D part profiles can be created from
our construction geometry using the Graphics
tool (inkwell pen) or the Hatch
For this example we want to create a closed
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"
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.
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.
The Dimension tool (also called "parameterization")
creates measurement constraints. It is
found in the top Command toolbar (again, with the 2D
still selected). It allows us to create dimensions in
our sketch to edit and change them by entering new
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
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
or press ENTER to apply the changed value. Sketch geometry
will be automatically redrawn with the new distance
value. (or click
or press ESCAPE to discard the change)
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.
"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
*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
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"
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
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
- T-FLEX uses both explicit geometry
(created by the user) and implicit geometry
(derived from existing shapes). Creating a new
drawing plane using the Workplane
tool is an
example of explicit geometry. Selecting a
flat side ("planar face") from existing 3D parts
as a drawing plane is an example of using
- If T-FLEX commands do not behave as
described, please check that you are not
currently still in a command. Use the ESCAPE key
to "back up" to the top level of the T-FLEX
design interface and try again.
1. We will create a new sketch using implicit geometry.
For this example you may need to activate face selection
by clicking "On" the "Select Faces" filter button
. Select the top face
of our 3D box.
It should highlight green. A context box will also
appear (shown right).
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.
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
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
contours (i.e. "regions") from construction
entities. Complex "Contour Autodetect"
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
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
modifies an existing "target"
with geometry applied from new "tool"
are combined into
complex models by either adding
to (like a
from (like a hole),
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).
start, we should now have a 3D box with an ellipse drawn
on top, as shown here left.
1. Select our ellipse profile. From the Context Box
select the "Extrude" tool (or right-click > "Create" >
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
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
. Your changes will be automatically
updated in the 3D model.
QUESTIONS OR COMMENTS ABOUT THIS TUTORIAL?