Dimensioning

Dimensioning enables you to describe geometry by displaying measurements. All dimensioning functions can be found on the Dimensioning toolbar or in the Objects / Draw menu. To create dimensions, select the objects to measure and drag the mouse to locate the dimension text (see Dragging Objects ). Dimensioning tools have several options for additional formatting and settings.


If dimensions are created in 3D views exported into 2D area, connections between dimensions and corresponding 3D objects are established. After changing 3D geometry and returning back into 2D mode, dimensions are automatically updated. See Automatic updates of dimensions, axes and hatches after changes in 3D


Once created, the dimensions can be easily edited (see Editing Dimensions ). Format and style of dimensions and dimension text can be modified using Dimension Attributes. Changing dimension text height affects the length of leader lines arrows.


Single Dimensions - Horizontal, Vertical and Diagonal

Horizontal Dimension - HDI
Vertical Dimension - VDI
Diagonal Dimension - SDI

Single dimensions are defined by selecting start and end points, then locating the dimension text.

Change Dimension Shape - Before the text location is defined, you can change the current dimension format. You can also use Dimension Format to set the format of future dimensions.

Dimension Format provides the following options:

  • Center dimension text - for the current dimension, all texts will be automatically centered. If turned on, this option turns centering off.
  • Toggle points and arrow - switches between points and arrows on the leader lines. This option is useful when space is limited.
  • Cancel predefined level - cancels all other previously selected options, the dimension is created at level exactly defined by cursor location.

These options of Dimension Format allow you to define the level (text location and dimensioning line location) of created dimension or all future dimensions:

  • Created dimension at the same level as selected (according to a selected dimension)
  • All dimensions at the same level as selected
  • All dimensions at the same level as created (next dimensions are according to the currently created dimension)
  • Created dimension parallel to selected
  • All dimensions are parallel to selected
  • All dimensions are parallel to created

The last option from menu allows you to redefine the dimension style.


Dimension arrows changed


Change Dimensioning Scale

Dimension scale value multiplies measured values of linear, diameter or radius dimensions. It must be used, if a part of 2D drawing is created in different drawing scale than entire drawing (for instance, in case of enlarged details).


Change Text or Tolerance - modify the dimension text or tolerances.

Dimension text is created automatically, and you can use Dimension Attributes to define its parameters. For currently created dimension, you can change text in the text input window.


You can select this option by clicking the corresponding icon in toolbar, from pop-up menu (available by default after Ctrl + Right-click), or, very conveniently by pressing TAB during dimension text location. The last possibility allows you to easily select the input text field, if you press TAB repeatedly – input is changed from dimension text to upper, then lower tolerance.

Dimension text window offers you to enter special characters, by clicking the corresponding icons. Also, you can click parentheses icon – then, entire text is closed into parentheses. Dimension text is properly updated after changes and remains closed in parentheses, too.



Change dimension text window


Predefined Horizontal, Vertical and Diagonal Dimensions

Predefined dimensions contain standard text characters such as diameter symbols. These are useful when dimensioning objects like circles or threads.

Horizontal Diameter Dimension - HDM
Vertical Diameter Dimension - VDM
Diagonal Diameter Dimension - SDM
Horizontal Thread Dimension - HTH
Vertical Thread Dimension - VTH
Diagonal Thread Dimension - STH

Example of predefined dimensions


Serial, Parallel and Datum Dimensions

These functions create multiple dimensions. The first dimension in this group is defined as for single dimensions (by 2 points), and subsequent dimensions in the group require only one point.

Parallel dimensions are a group of dimensions that all start at the same point. The offset between parallel dimensions is defined in Dimension Attributes. Datum dimensions consist of a line of points, at each of which the dimension defines the total distance from the start point. Serial dimensions are a chain of aligned dimensions that define the distance from point to point.

Horizontal Parallel Dimensions - HPD
Horizontal Serial Dimensions - HSD
Horizontal Datum Dimensions - HDD
Vertical Parallel Dimensions - VPD
Vertical Serial Dimensions - VSD
Vertical Datum Dimensions - VDD
Diagonal Parallel Dimensions - SPD
Diagonal Serial Dimensions - SSD
Diagonal Datum Dimensions - SDD

Example of baseline, serial and datum dimensions


Angular Dimensions

Angular Dimension - ADI

Angular dimensions define the angle between two lines. You have the same additional options for dimension shape changes as for the linear dimensions. See Change Dimension Shape.


For angular dimension, define first and second line. When the second line is defined, you can optionally select following:

Greater Than 180 - dimensions the angle greater than 180 degrees.
Turn off dimensioning of angle greater than 180 degrees, cancels the previous mode.
Complementary Angle On - dimensions the angle complementary to 180 degrees.
Complementary Angle Off - turns off the complementary angle dimensioning, cancels the previous mode.

Example of default angular dimensioning, complementary angle dimensioning and dimensioning of angle greater than 180 degrees


Diameter and Radius Dimensions, Thread Dimensions

Radius Dimension - RDI
Diameter Dimension - DDI

These dimensions are defined by selecting an arc or circle and locating the dimension text. Additional options for radius dimensions are:

  • Extend to radius center - creates a mark at the arc center.
  • Not to extend to radius center – cancels the previous mode.

Thread dimensions - THR
Horizontal Thread Dimension - HTH
Vertical Thread Dimension - VTH
Diagonal Thread Dimension - STH

Thread dimensions behave like diameter or linear dimensions, except the predefined thread symbol is used. If the thread is created in 3D and then exported into 2D, either in sections or in a view, the dimension text is created automatically according to corresponding 3D object. Dimension recognizes thread type (like Metric thread, Pipe thread), and thread size or pitch (like M10, M10x1 …). It is necessary to use these four dimensioning commands to obtain the corresponding thread text, according to creation in 3D. Also, threads should be exported to 2D from basic views (like front view, back view, top view…).


Single Text Arrow - STXA

Creates a text connected to a single arrow.

Multiple Text Arrow - MTXA

Creates multiple lines of horizontal text connected to an arrow.


Example of text connected to an arrow


Dimension Attributes

Dimension Attributes - DMA

Available on the Tools menu, Dimension Attributes enables you to change dimension styles and other properties. The following properties can be modified:

  • Text attributes - height, slant, width and font. Text height controls the size of leader arrows.
  • Dimension text format – number of decimal digits, usage comma instead of period, inch values format
  • Size, overlaps, tolerances - distance between parallel dimensions, distance between text and leader lines, witness line creation, tolerance position
  • Angular dimensioning
  • Arrow style
  • Text prefix or suffix – defines usage of radius, diameter or thread marks

Changing dimension attributes allows you to set dimensioning according to various drawing standards, like DIN or ANSI. Dimension attributes are used also for finish symbols or single or multiple text arrows.


Edit Style of Selected Dimensions - EDS

This command changes the style of selected dimension or dimensions (also from entire drawing) to a style of a selected dimension, or according to current dimension style settings.



Dimension style settings


Example of dimension styles


Finish Symbols

Finish Symbols - FSY

Finish symbols are created by entering a roughness value, or by selecting a symbol for not-machined surfaces. Symbols can be attached to a line, arc or dimension witness line, or they can float. When attaching to a 2D object, you can drag the symbol around the object before selecting its final position.

Finish symbols example


Weld and Tolerance Symbols

Weld Symbols - WSY

The weld symbol includes a basic symbol, supplementary symbol, dimension of weld size, and weld process symbol. When defining a symbol, you can change text and other attributes, and see a preview before creating it. You can also save up to nine symbols for future use. To create a weld symbol, first select the weld location and then select the symbol location.



Welding symbols definition


Example of welding symbol; this symbol was created within one function.


Weld Symbol Settings - SWS

Available on the Tools menu, allows you to choose whether the weld symbols will be created according to ISO or ANSI standards.

Tolerance Symbols - TSY

Similar to welding symbols. Datum feature symbols can also be created.



Tolerance symbols definition


Creating Leaders, Item Numbers

VariCAD has a complex system solving item numbers and their appearance in 2D leaders. If BOM mask contains an attribute prototype of type “Item Number”, you can define item numbers of solids together with other solid attributes. Moreover, you can define item numbers in BOM. Here, you may define item numbers for a batch of objects, or for entire assembly at one step. Also, you can remove item numbers the same way. See Defining Item Numbers in BOM section for more information.


If once defined, item numbers are exported to 2D drawings together with corresponding 2D views of 3D solids. In 2D, during leader creation item numbers are detected automatically from 2D objects.


If you change item numbers in 3D solids and if you perform a new export of 3D views into 2D area, item numbers can be checked and updated automatically. If necessary, leaders can be easily deleted from entire 2D drawing or from a selected 2D region. Leaders can be selected as a sub-type of dimension.


Leader style in 2D can be modified as well as a style of dimensions. Leader style settings are part of dimension settings. Leaders themselves are sub-part of dimensions objects.


Create Leaders - LDR

This command creates 2D leaders. If 2D drawing was exported from 3D and if 3D solids have defined item numbers, leader texts (numbers) are assigned automatically to each leader. Otherwise, the leader number is assigned from 1 and each next leader has the number increased.


Following options are available during leader definitions:

Changes default text of the created leader.
Changes leader (or dimension) style.
Sets distance between adjacent leaders.
Creates temporary leading lines at the selected leader. This allows you to keep the next leader adjusted horizontally or vertically according the selected leader.
Leader witness line is a spline. This switches witness line creation from a single line to a spline.
Leader witness line is a single line. It turns off witness line created as a spline.


Leader style definition, text style



Leader style definition, text side of leader



Leader style definition, object side of leader


Example of leaders


Editing Leaders

To change existing leaders, right-click a leader and select action from pop-up menu.

Edit leader. This allows you to change leader shape the same way, as it is created.
Edit leader text.

Checking Leaders, Updating Leaders

If you defined item numbers in 3D and a 2D drawing containing leaders was created, you can change item numbers in 3D again. In 2D drawing, leaders are correctly rewritten or checked by following command:


Check and Update Leaders (Item Numbers) - CHLDR

If there are leaders to be updated, following dialog appears:



Update leaders


After confirmation, leaders are correctly rewritten and optionally highlighted. Highlighting of updated leaders is turned off by calling the update command again.


Editing Dimensions

Edit Dimension Text - EDI

Edits the text of a selected dimension. The same text editing options are available as when you created the dimension.

Move Dimension Text - MDT

Uses drag and drop to move the text of a selected dimension. Be careful when using this function, because if you create more dimensions after moving the text, you could have overlapping objects.

Edit Dimension - EDM

Change any attribute of a dimension. You can change everything about a dimension except for the original dimension definition points or the 2D dimensioned object. Dimension shape is defined the same way as if you create a new dimension. Similarly, you can change style, text or dimension shape.


 

 


VariCAD HELP

Introduction to VariCAD
VariCAD Installation Installing Upgrades Hardware and Software Requirements
Files and Directories Used by VariCAD Default VariCAD Files Converting 2D/3D Objects to and from Other Formats How 3D Objects Are Converted to STEP or IGES Creation of STL format Directories
Getting Started VariCAD User Interface Working with Multiple Monitors 2D/3D Area Status Bar Toolbar Icons Dialog Windows - Cancel and Back Buttons Mouse Buttons 3D Mouse Invoking and Running VariCAD Functions Finishing VariCAD Functions Stepping Back within a Function Selecting Objects between Functions Additional Options within Functions Creating, Opening and Saving VariCAD 2D/3D Files File or Folder Preview Definition Backing up Your Files Working with Multiple Files Copy and Paste Switching between 2D and 3D Undo and Redo Dragging Objects Dragging Increments Turning off Detection Temporarily
System Settings (Preferences) Backing up Your Configuration Colors
2D Drawing Displaying the 2D Drawing Area Changing the View Using the Mouse and Keyboard Display Functions Rebuilding Functions Zoom Functions Saving Views 2D Display Settings 2D Circle Display Settings Cursor Settings and Coordinate Listing Types of 2D Objects 2D Drawing Attributes - Units, Formats, Scale Units Format and Sheet Border 2D Drawing Scale Attributes of 2D Objects Working with 2D Layers 2D Object Colors Line Types Visibility of 2D Objects Work Sets 2D Coordinate System
2D Drawing Aids Grid Construction Lines Creating Construction Lines Deleting Construction Lines Creating Multiple Construction Lines Temporary Construction Lines Transient Construction Lines Increment Cursor Mode Ortho Mode
Selecting 2D Objects Using Selection Windows Limited 2D Selections Deselecting Objects Finishing the Selection Selecting 2D Locations Defining Angles and Directions Writing Special Characters Mathematic Expressions Checking Objects, Distance, Angle and Coordinates
Drawing 2D Objects Drawing Lines Arrows Drawing Curves Creating Points Creating Circles and Arcs Creating Text Objects Editing and Deleting 2D Objects Deleting Objects Changing Objects Geometry Creating Corners, Chamfers and Fillets Breaking and Dividing 2D Objects Editing Text Transforming and Copying 2D Objects Translating, Rotating and Scaling Mirroring Objects Offsetting Objects Stretching Objects
Dimensioning Single Dimensions - Horizontal, Vertical and Diagonal Predefined Horizontal, Vertical and Diagonal Dimensions Serial, Parallel and Datum Dimensions Angular Dimensions Diameter and Radius Dimensions, Thread Dimensions Dimension Attributes Finish Symbols Weld and Tolerance Symbols Creating Leaders, Item Numbers Editing Dimensions
Axes
Hatching Solid Fill Hatching 2D Objects Editing Hatches Creating a Hatch Pattern
Symbols 2D Blocks Creating and Inserting Blocks Editing Blocks 2D Polylines Creating Polylines Editing Polylines
Automatic Updates of Dimensions, Axes and Hatches after Changes in 3D. Automatic updates of dimensions Automatic Updates of Axes Automatic Updates of Hatches Checking of Updatable 2D Objects and Dimensions
Libraries of Mechanical Parts Selecting Mechanical Parts Configuring Mechanical Parts Selection Dialog Inserting Mechanical Parts into 2D Inserting Mechanical Parts into 3D Pre-selecting Dimensions Options Available for Mechanical Parts in 3D Modifying Mechanical Parts in 3D Modifying Counter-parts, Drilling Holes for Screws Mechanical Part Calculations
Printing and Plotting Printing Methods Selecting a Printer Batch Print Exporting Images as Bitmaps
VariCAD on the Internet Trial Versions, Online Purchasing
3D Display Dynamic View Manipulation Animated View Changes Predefined View Rotating View Using the Arrow Keys 3D View Tools Saving Views Shaded and Wireframe Display 3D Display Settings View Rotation Center Enhanced Rendering Surface Shading Setting 3D Display Performance Hardware accelerated OpenGL Test of Hardware Performance 3D Objects Shape Representation Types of Shape Representation Converting Shape Representations into Different Types Highlighting Objects with Open Surfaces Solving Problems in 3D Tools Rebuilding 3D Data Structures Tools Repairing Erroneous Solids Loaded from STEP Tools Repairing Erroneous File Sketching - 2D Drawing in 3D Planes, Drawing Methods Displaying Objects 2D Drawing Features Construction Lines, Temporary Construction Lines Working with 3D Objects
Creating Solids Sketching of a 2D Solid Profile Sketching Plane Definition Sketching Environment, Finish Sketching Sketching of Profile of New Solid Displaying of Created or Edited Solids Multiple Sketching Planes Common Sketching Features Additional Sketching Features Closed Rotation of Multiple Profiles Convergence of Lofted Profiles into One Point Tangent Direction of Lofting Features Related to Solid Creation Method Manual Selection of Profile’s 2D Objects Solid Insertion Point Solid Insertion Point for Profiles Selected in 2D Mode Rotating, Extruding, and Lofting Profiles Rotated Solids Extruded Solids Lofted Solids Helical Surfaces Basic Solid Volumes Cylinders, Cones, Boxes, Pyramids, Pipes, Spheres Editing of Spatial Dimensions of Basic Solids
Editing Solids Selecting Solids Visibility of 3D Objects Shading and Colors of Individual Solids Boolean Operations - Adding and Cutting Solids Boolean Operations Boolean Tree Structure Editing Common Boolean Operations Holes, Grooves, Cutting by Planes Resolving (Exploding) Solids 3D Filleting and Chamfering Deleting Solids Editing Shape of Solids Edit Solid Element Shape Transforming and Copying Solids Solid Object Coordinate System 3D Space Coordinate System Inserting and Transforming Solids Defining Vectors and Rotation Axes Transforming Objects Using their Axes Translating by Distance Dynamic Translation Rotating by Angle Dynamic Rotation Dragging in Increments Additional Rotation around an Axis Setting the Direction of Solids Axes Positioning and Location at Surface Positioning by Plane Zoom in on Transformed Solids Additional Options for Right-Click Objects during Transformation Additional Boolean Operation, Constraints Definition Changing Insertion Point, Displaying Axes Inserting and Copying Identical Copies of Solids Permanent Change of Axes of Solids Imported from Step Defining 3D Locations Selecting Planes 3D Locations Settings Mirroring and Rescaling Solids Exploded View of Assemblies Groups of Solids
Parameters Definition of Parameters Parameters in File Parameters in Scaled Solids Type of Parameters Working with Parameters Geometric Constraints Constraints as Additional Transformations Constraints as Removed Degrees of Freedom Definition of Constraints Constrained Objects Types of Geometric Constraints Chain of Constraints Fixed Object within Constraints Constraining Angles Constraints in Solid Creation 2D Profiles Constraining Objects in 2D Profile Selecting Vertexes Display Options Filleting, Chamfering and Radii of Circles or Arcs Constraining Circular Arcs Constraining NURBS Curves Editing Constraints Deleting Constraints Coordinate Systems
Exporting Views and Sections from 3D to 2D Creating 2D from 3D List of 3D View Exports, Updating Views 3D Sections 3D Comprehensive Shapes Creating and Editing 3D Texts Pipes and Wires Sweeping of 2D Profiles Offset Patches – Thick Shells Threads in 3D
Checking Functions and Calculations Units of Calculation Results Volume, Mass, Surface and Moment of Inertia Calculations Checking and Measuring Geometry Interferences among Solids
3D Assemblies Creating Part Files, Assembly Files and Assembly Links Saving and Loading the Assembly Files Sub-assemblies Relative Paths in Assembly Links Simultaneously Open Assembly and Part Files Definition of Assembly-Part links Definition of Sub-assembly - Part links Breaking Links between Part or Sub-assembly and Assembly Editing Sub-assemblies or Parts in Assembly Environment Selecting Parts or Sub-assemblies for Editing Editing Parts or Sub-assemblies 3D Assembly Tree Scheme 3D Assembly Tree Scheme Window Objects Select Mode Part Editing or Attributes Definition Mode Managing All Assembly Tree Files Surface Development (Unbending)
Bill of Material, Object Attributes and Title Blocks Object Attributes BOM, Attributes and Title Blocks Mask Sharing BOM, Attributes and Title Blocks Settings (Mask) Attribute Definition Groups of Attributes Output to Formatted Text (List of Parts) Title Blocks Export to Other Systems Compatibility of Defined Attributes and Attribute Groups Working with BOM BOM at Basic Level BOM Containing structure of Assembly BOM from 3D Group BOM Objects Displaying, Filtering and Sorting BOM Objects Creating Files from BOM Copying Data from Assembly into Parts and Vice Versa Defining Item Numbers in BOM Single Click Attributes Copy Attributes from 2D Area Supplementary Objects Solid and Assembly Attributes Solid Attributes List of Materials Material as a Solid Attribute Assembly Attributes, Title Block Filling
Tips and Tricks List of All VariCAD Functions Hotkeys Embedded Functions

QUICK DEMO

Tips and Tricks
Basics Of Control

Interface, examples of various input steps, like mouse button clicks, hot-keys and their combinations. Examples of detection, objects selection and view changes.

Tools for 2D location, Tool combinations

Tools for location of 2D objects.

2D object selection, Filter combinations

Tools for selection of 2D objects.

Line

Drawing line from a point to another point, Using leading lines, According to values entered from a keyboard (xy, dx dy, angle radius, called by pressing K, D, R keys), Using fixed (locked) values (called by pressing TAB key), Combining multiple tools (TAB, dxdy...), Tangent lines.

Rectangle

Drawing rectangle by two opposite locations, Using fixed (locked) values (called by pressing TAB key), Diagonal distance.

Multi-line

Offset at one side from the central polyline, Offset at both sides from the central polyline.

Circle

Drawing circle by center and point at the circle, Center and radius, Two points, Three points, As a tangent to 2 objects, As a tangent to 3 objects.

Rotated parts

Shaft – a front view, Shaft – create a contour.

Polygon: hexagon

Leading circle is inside, the polygon orientation is at the edge, Leading circle is outside, the polygon orientation is at the vertex.

Dragging a circle to the rectangle center

Dragging, start by Ctrl+Shift+move cursor over an object, Dragging – right click. Two methods, different location at a center, Dragging, clicking an icon, Using Ctrl+X, Ctrl+V, Translate by a defined vector, Translate to a shifted center, Locate, using incremental cursor movement.

Stretching of objects

Dragging, start by Ctrl+Shift+move cursor over an object, Dragging – right click. Two methods, different location at a center, Dragging, clicking an icon, Using Ctrl+X, Ctrl+V, Translate by a defined vector, Translate to a shifted center, Locate, using incremental cursor movement.

Blending

Filleting of 2D corners, instant access (using Shift key), Filleting of 2D corners, Chamfering of 2D corners, instant access (using Shift key).

Divide or extend a 2D object

Extend to a boundary, Create a full circle from a circular arc, Remove a segment, Trim, Divide an object by a boundary, Divide an object by a point.

Changing 2D object attributes

Changing color, Changing line type, Changing layers, Blank/unblank objects (invisible/visible), Changing displayed thickness - 1 or 2 pixels.

Dimensioning

Smart dimensioning – easy dimensioning done within a single command. Horizontal and vertical dimensioning. Dimensioning of threads, chamfers, fillets and diameters. Aligning dimensions according to each other.

Settings

Drawing format, sheet border, Drawing scale, Using 2D layers, automatic changes of 2D layers, Default settings of a new file.

Creating a 2D drawing data

Drawing 2D objects and filling title blocks manually in the 2D area, 2D objects and title blocks created automatically from 3D space, Printing to PDF.

Selection of solids

Working with 3D solids. Examples of solid insertion, selection or transformation.

Solid transformation

Examples of solid insertion, detection and transformation. Examples of solid copying.

Single solid shapes

Creating predefined solid shapes (Box, cylinder, cone, pipe...). All solids can be created by rotation, extrusion or lofting of contours.

Solid creation by defined contour

Solid creation by extrusion, full or partial rotation of contour.

Lofting rectangle to circle

Creating a solid by lofting rectangle to circle.

Lofting a rectangle to single point

Creating a solid by lofting a rectangle to single point.

Lofting among multiple contours

Creating a solid by lofting among multiple various planar profiles.

Lofting among profiles rotated symmetrically around an axis

Creating a solid by lofting among multiple various planar profiles.

Sweeping of a 2D contour in 3D space

Sweeping of a 2D contour - creation of a banister, pipe...

Creating pipes or wires

Creating of pipes, wires (banister, cables, ropes...).

Rotation and lofting of contours

Rotation and lofting between two different contours, like between a circle and rectangle or between circles with different radii. Profile change is linear or allowing tangential direction from both ends.

Helical surface

Creating a helical surface by simultaneous rotation and extrusion of 2D contour.

Creating holes and grooves

Creating holes and threaded holes, cutting by an extruded contour, creating groove, cutting by a box. X axis of a tool is always perpendicular to selected surface.

Shells, sheet metal parts

Creating a sheet metal part using shell tools.

Editing of solid elements

Editing of solid elements by changing dimensions. Values can be defined in tables or by 3D dimensions. Editing of dimensions together with change of location of solid elements.

Editing of solid elements by changing creation contours

Editing of basic shapes by changing their creation contours.

Editing of solid elements, selection by cursor or from scheme

Solid element can be selected by cursor (press and hold Ctrl key, move cursor over it), or from Boolean tree scheme.

Editing of 3D pipes and wires

Example of creation of 3D wire, thread and geometrical constraint. Next step shows editing of it.

Assembly, Parts, 2D Drawings

An example of alternative creation of an assembly, sub-assembly, parts and corresponding 2D drawings.



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