Basics of Catia Drafting

Intro to Drawings

Always make contact, as early as possible, with the person(s) who will be doing the checking of your drawing before you begin.  Do not wait until you start the drawing.  Check with these people before you even start the task.  Do not underestimate this advice.  There are often particular ways individual teams and personalities will want your drawing to conform to.  Try to make this work to your advantage by conforming to their way and perhaps a little flattery wouldn’t hurt either. 

BOM

            Defining BOM appearance

            Inserting BOM in Drawing

            Post Insertion BOM Editing

            Preparing the models for the BOM

Defining BOM appearance

While in Assembly mode (double-click on your assembly), select the Analyze pull-down menu, Bill Of Materials, select “Define formats” button, add to the “Displayed properties” field with the |< icon; remove a property from the “Displayed properties” field with the |> icon.  For example, the following may be in the left hand column: Quantity, Part Number, Nomenclature, Definition, Revision, Number.

See Post Insertion BOM Editing for other detail regarding renaming Displayed Properties

Inserting BOM in Drawing

See Preparing the models for the BOM to prepare the Parts/Assemblies for the BOM.

While in your BOM drawing sheet(s) place the BOM into the sheet’s Background as described below. 

The BOM will first be inserted while in “Working View” mode (Edit pull-down menu should say Background at the bottom) then Cut from the “Working Views” so that it can be Pasted onto the Background of the sheet.  The assembly selection step will be a similar process as that described in View Creation Wizard (Open your drawing, open your top assembly…).

Insert, Generation, Bill of Materials, Window, Tile Horizontally, select the assembly from the Tree (in the Assembly file), pick a spot on the drawing sheet where you want the BOM (wait for an approx. 5 second delay).

Then select the BOM, Cut (Ctrl-X), Edit, Background, Paste (Ctrl-V) onto the Background.

See Printing – Display Print Area to print out a rough copy of the entire BOM.

Back to Post Insertion BOM Editing

Post Insertion BOM Editing

Double-click on BOM that was placed on the Sheet to enter modification mode.  Before spending time “tweaking” the BOM make sure you’ve spent adequate time with Preparing the models for the BOM and Defining BOM appearance.  Run some reference copies (see Printing – Display Print Area) for whoever will be checking your drawing before conducting these “post insertion edits” so that the “Post Insertion BOM Editing” will indeed be on your final iteration.  This is important since these “post edits” will be lost if you ever decide that another “Inserting BOM in Drawing” is necessary.

While in modification mode:

            -Double click on any text to modify it

            -Drag the “squiggly” row/column indicators to move the columns/rows.

Back to Defining BOM appearance

Preparing the models for the BOM

Recommended to open part files in their own window before populating the below “Product” fields.  But if you do decide to perform in your assembly file make sure that you expand  the component branch so you apply the following to the parts/assemblies and not the components. 

Once a part is assembled to an assembly it is a component.  Expand  the component to see its indentured part or assembly. Right-click on the part or assembly and select Properties.  The Product fields (within the Product tab) will populate the BOM.  The recommended fields to use are:

            -Part Number

            -Definition

            -Nomenclature

            -Source

Additionally the “Visualize in the Bill Of Material” radio button should be selected.

See Defining BOM appearance.

IMPORTANT: Read and understand Save Management.  After completing the input to the above Product fields make sure that Save Management is reporting that the files have been “Modified”.  If Save Management only says that the file is “opened” then you will have to perform something to coax the file as modified (e.g. open the part in it’s own window, double-click on one of its sketches and immediately exit the sketch, close the part and if Catia notices it was changed it will ask you if you want to save it.  You can answer Yes or No (to this window) but I would suggest answering No and track all of your “Property edits”/”save verification” with the Save Management method as described above.  This way you can more easily track which Property edits will require additional “coaxing” until Save Management shows “Modified”.  When you are finally confident that all of your parts (that had their Property “Product fields” edited) will save, save your top assembly (the assembly that all of your parts feed into) and all of your parts/assemblies should save with it.  Reopen Save Management afterward to verify that all parts have saved (their State would have changed from Modified to Opened).

Back to Inserting BOM in Drawing

Back to Post Insertion BOM Editing

Drawing Format Help:

            Adding Format (into existing drawing)

            Resizing Page (Page Setup) For Fitting Format

Adding Format (copying from one drawing to the other):

            Copying a format – Method 1 (out of an existing drawing)

            Copying a format – Method 2

            Pasting a format

            Editing the format

Copying a format – Method 1 (out of an existing drawing)

Open our drawing (h drive link shown below) where we have dedicated sheets for all of our standard formats, arrow  over to see other sheets (tabs), take note to Page Setup (e.g. w=120, h=34.5), Edit, Background, select all by using the rectangle selection trap , Copy (Ctrl-C), (Or see Copying a format – Method 2).  See Pasting a format for pasting the “Cut” geometry.

-Return to your working views by selecting: Edit, Working Views.

Copying a format – Method 2

Make sure you’re in “Background” mode (i.e. Edit, Background), File, Page Setup, select “Insert Background View” button, select Browse, browse to the drawing (e.g. template drawing) where you’d like to import a Background from an existing sheet, Open, navigate to the desired sheet in the Sheet pull-down  menu, select Insert, OK.  Only the Background from the “template drawing” will be imported. 

-Press Undo (Ctrl-Z) if results were undesirable.

-Exit Background mode (Edit, Working Views).

Pasting a format (out of an existing drawing)

See Copying a format.  Open the drawing that you want to paste into (if already open use Window pull-down menu), Edit, Background (no views should be highlighted red), Paste (Ctrl-V).

-Return to your working views by selecting: Edit, Working Views.

Editing the format

Assuming the format was added to correctly (to the Background) as defined in Adding Format, Edit, Background (no views should be highlighted red), double click on each text to edit.

-Return to your working views by selecting: Edit, Working Views.

Resizing Page (Page Setup) for fitting Format:

While in a Drawing do the following for each Sheet: File, Page Setup, enter appropriate values in the Width and Height fields (e.g. select “J U.S.Standard” from Format field, and enter 120 in Width field, 34.5 in Height field) as described in Standard drawing format sizes, Resize  the drawing. 

See Move multiple views.

Text & Callouts

            Considerations when adding to views

            All around symbol

            Create interruptions (extension line break)

            Scribe lines and markings

            Weld Symbols

Considerations when adding to views

Always activate the desired view before adding text.  This assures that text will be added to the anticipated view and the text will remain in the anticipated position during moving of views.  If the desired view is not activated than the current active view will automatically (and inconspicuously) expand its view border to include the new text.

Activating a view (view border becomes red) by one of the following methods:

-Double Click on the view border.

-Right-click on the view border (or on view name in the Tree), select Activate view.

All around symbol:

highlight the leader, right click on yellow ball  (at the end of the highlighted leader), select All Around.

Create interruptions (extension line break)

(so dimension extension lines break so as not to run over a dim. Arrow),

-right click on a dim., dimensionname object , Create Interruption(s), select on two locations on the extension line to define the break.

Scribe lines and markings:  

make a dedicated sketch, right click on the drawing view that will show the sketch geometry, Properties, check the “3D Wireframe” bullet and the “3D Points” bullet, OK.

Weld Symbols

            Making a Weld Symbol

            Modifying a Weld Symbol

Making a Weld Symbol

Insert, Annotations, Symbol, Weld Symbol, click on the screen to define the arrow location, click twice on the screen to locate the symbol, select the appropriate symbols, OK…

Modifying a Weld Symbol

Double click on weld symbol…

Printing

            Printing – Display Print Area

            Printing reduced size prints

            Standard drawing format sizes

Printing – Display Print Area

Ctrl-P (or File, Print), change to the desired printer (in the Printer Name: field), change the Print Area pull-down menu to Display, select the “Fit to:” bullet (Position and Size section), select Page Setup button, change Width to 11, change Height to 17 (for a 11”X17” vertical printout), OK, select the Preview button, if the preview clips some of the BOM continue with step 1 below if not continue with step 2:

1. OK (to exit Preview), select the Center button, adjust the Scale field, hover the cursor over the gray rectangle (with the “X” thru it) and drag the region to a new center, select Preview  button again and judge again, repeat or proceed to step 2.
2. OK (to exit Preview), OK to send to printer.

Back to Inserting BOM in Drawing

Back to Post Insertion BOM Editing

Printing reduced size prints

Keep reduced size prints proportional to the actual drawing format size.  Use the Measure icon to measure the length of the drawing border.

Ctrl-P (or File, Print), change to the desired printer (in the Printer Name: field), change the Print Area pull-down menu to “Whole Document”, select the “Fit in Page” bullet (Position and Size section), select Page Setup button, change Width to 11, change Height to 36* (for a 11”X36” horizontal printout), OK, select the Preview button (all of the drawing should be within the red dotted lines), OK, OK.

*Example: for a 66” long J size (H=34”) print at ½ size: print at W: 33 H: 17, fit to page

(W: 36, H=11 seems to work well for many plotters [for J sizes up to 120” long] and is legible).

Standard drawing format sizes

A: 8.5 x 11

B: 11 x 17

C: 17 x 22

D: 22 x 34

E: 34 x 44

J: 34 x 55min (176 Max)

Drawing Views

            Adding Views

            Drawing Views icon group

            For view maintenance purposes:

            Modify Dimensions (Right-click on dimension, Properties,…)

            Modifying Views

            Move multiple views

            Move views to other sheets

            Selecting views

Adding Views

            Adding Projection View

            View Creation Wizard

Adding Projection View (to existing view)

See Drawing Views icon group for location of Projection View icon and other “Projections” group icons.

Activate (double click on) the parent view (activated view border should be red), select the Projection View  icon, move your cursor to the desired position (close to the activated parent view), left-click to accept view location.

View Creation Wizard

Review For view maintenance purposes.

See Drawing Views icon group for location of View Creation Wizard icon and other “Wizard” group view creation icons.

Open your drawing, open your top assembly, Window, Tile Horizontally, select the View Creation Wizard  icon (if grayed out you haven’t opened your top assembly), select one of the Configurations icons on the left (e.g.  “Configuration 1 using the 3^rd angle projection method”), Next, select another icon on the left (if additional views are desired), Finish, This next step is important if you want to link directly from the drawing to the top assembly only: select a component from the Tree (preferably from the 1^st instance [e.g. componentname.1; for commonality sake] if more than one instance exists) before selecting a planar surface, right-click the component you just selected from the Tree and select “Reframe on”, now select a planar surface from the highlighted component in the graphics window, next do one of the following:

-click anywhere on the screen (except on the “view orientation” arrows) to accept the default orientation

-or click on one of the large arrows to flip the view orthogonally

-or click on one of the two curved arrows to rotate the view about an axis normal to the sheet

Back to Inserting BOM in Drawing

Drawing Views icon group

Back to To save the view (adding custom views)

Back to Adding Projection View

Back to View Creation Wizard

Back to FTA & Drawing views

For view maintenance purposes:

Note: You can use your top assy always as the assembly to pick the planar face of the view.  But the key is to first select the model (part/assy) from the top assembly’s Tree, then pick the planar face from the graphics window.  This way when you go to “File, Desk” it shows links from the drawing view directly to the top Product.  This is often the preferred linkage.  Often preferred to have the drawing directly linked to the top product only (see Desk).

The following (along with Removing components from view) assures that proper view Updates with the minimum amount of view maintenance.

-View creation should be from the smallest model (least number of parts).  Thus, for a view showing a single part, the planar surface selected to define view plane should be from a part file (.CATPart).  For a view showing an assembly, the planar surface selected should be from the pertinent sub-assembly (so as to minimize manually clicking off the radio buttons as described in “Removing components from view” below).

- Unlocking a view (right-click, Properties, uncheck the “Lock View” radio button (under View Tab)

Selecting views:

-Select them (left-click) from the Tree, although they can be selected by the view borders

-Multiple view selection in the Tree: select first view (at top of list), hold the Shift key as you select the last view (bottom) in the Sheet’s Tree list.

Back to Move multiple views.

Modify Dimensions (Right-click on dimension, Properties,…)

            Removing 2^nd Arrow

Removing 2^nd Arrow (e.g. for Ø callout)

Right-click on dimension, Properties, “Dimension Line” tab, uncheck the “Symbol 2” radio button.

Modifying Views

            Break a view – Broken View (compresses a view by omitting the middle geometry [between the breaks])

            Adding a break in a view – Breakout View

            Removing components from view

Break a view – Broken View (compresses a view by omitting the middle geometry [between the breaks])

See Drawing Views icon group for location of Broken View icon and other “Break view” group icons.

Activate (double click on) the parent view (activated view border should be red), select the Broken View  icon, follow directions in lower left of graphics window….

-Don’t forget you can use Undo (Ctrl-Z), repeatedly until the view returns to it’s “pre-broken” state, if undesirable results.

-To delete the Break, right-click on the break (so it highlights), Delete.

Adding a break in a view – Breakout View

Activate (double click on) the parent view (activated view border should be red), select the Breakout View  icon, define a breakout loop by left-clicking (multiple points) on the portion of the view to be broken (see lower left of graphics window if further direction is needed), double click to end definition of the breakout loop.

-To remove breakout: right-click on the view, viewname object >, Remove Breakout.

Removing components from view:

Right-click on view, viewname object > Overload Properties, select the component (that is to be removed) in the view, Edit, uncheck both of the following two radio buttons: “Use when projecting” & “Shown”.

Move multiple views:

See Selecting views.  After the views have been selected (geometry will be highlighted in each view) initiate the move by depressing & holding the left mouse button atop one of the view borders (away from any entities), drag the depressed left-click to the new location on the sheet.

-Other view movement options are available by right-clicking on a views border and selecting View Positioning.  For example, select two views (with Ctrl key), right-click on view border, View Positioning, Element Positioning, place cursor over the variety of Align options, select the

Back to Resizing Page (Page Setup) For Fitting Format

Move views to other sheets: select the view from the Tree, Cut (Ctrl-X), select the sheet that the view will be moved to and Paste (Ctrl-V).  Recommended to move the views to an anticipated “empty” location (if convenient) so that once they are moved to the new sheet they won’t be atop other views.

Creating a new part in an assembly:

Creating a new part in an assembly:

Running example 1:

To add (and create) a part “on the fly” while in the assy: select the New part Icon, , then select the assembly (in the Model Tree) that the component (new part) will be added, enter the new part number in the pop-up window, Answer No to the following question: “Do you want to define a new origin point for a new part” (this assures that the new part being created will also come in “rigged” [i.e. in position relative to the common csys]).

Note: to start working on the part within the assembly: expand the  sign next to component (to see the part underneath it) in the Tree, double click on the indentured part (to enter into Part mode); the  PartBody should be the “Defined in Work Object” (i.e. underlined).  To continue making a part see Part (Running example 2).

Back to Running example home

Creating a sub-assembly in an assembly

Double-click on the assy (enters into Assembly Mode for that assembly) that you want to add the new sub-assembly to, click on the Product  icon, select the parent assembly again if it asks you to, type in the new part number.

See also Moving/Copying a part to another sub-assembly.

Adding Components:

            Adding commonly “rigged” Components:

            Adding non “rigged” Components (aligned with other geometry):

            Replace Component

Adding commonly “rigged” Components:

Use “Existing Component” icon: , select the assembly in the Tree that the component will be added, select component from pop-up window, Open.

See Assembly Constraints Icon group if further constraining (aligning of parts) is required.

Adding non “rigged” Components (parts that need to be aligned with other geometry): Use “Existing Component with Positioning” icon: , select the assembly in the Tree that the component will be added, select component from pop-up window, Open (a new window will open; use same View Orientation controls [i.e. zoom, pan…] in either graphics window), select a constraint type from the “Quick Constraint” menu, follow element selections similar to that for Smart Move.  A  branch will appear in the Tree which will hold the component’s constraints.

Back to File, Save As

Replace Component

Right-click on the component (in the Tree), Components, Replace Component*, browse to location of the “new” file and select it, Open, consider and answer the “yes or no” question (Do you want to replace all of the instances of the selected element ? [select No if you want to only replace the one you picked and not all]), OK.

Note: Finding parts per Search example can be very helpful (when replacing components) to assure that all of a part’s/component’s “Instance names” (under Properties) are representing the new part.

*or you may select Replace Component In Session (if the replacement part is already in session and you desire a convenient list of only the parts that are in session).

Back to Save As – one Part considerations

Move Icon Group (Assembly)

            Manipulation Parameters window

            Snap icon (align without constraints)

            Smart Move (align components with multiple constraints)

-Before initiating the move, whose top indentured components you want to move, the assembly must be highlighted blue and in Design Mode. :

Note 1: Some “best practices” avoid constraining their components and instead prefer creating & assembling parts/assemblies per the Adding commonly “rigged” Components method.

Note 2: Consider using an associative approach by using the Constraints Icon group (Assembly) for an alternative to the Move icon group.  The constraints method would maintain an associative link between the components.

Note 3: Recommended to check external relationships of the component to be moved first to see if other parts would follow it in the reposition.  Do this by utilizing the Dependencies under the Analysis pull-down menu.

Manipulation Parameters window

Example:

-To activate the assembly, whose top indentured components you want to move, double click on it until it remains highlighted blue. Single-click on another component to un-highlight the assembly to see that it remains highlighted blue.

Select the Manipulation  icon, select the “Drag along any axis”  icon, select an edge that will represent the direction axis, select the component to move in the graphics window, left-click and drag (hold down left mouse button as you move cursor) to desired position,  press OK to accept final position.

Snap icon :

Double click on the assembly (which is the parent of the component to be moved) to activate it.  Select the Snap icon, follow the directions in the bottom left of the graphics window (will define what you should be selecting).

Smart Move  (align components with multiple constraints):

Select the Smart Move icon, check on the “Automatic constraint creation” box, select a constraint type from the “Quick Constraint” menu, select an element on the first component (e.g. point, line or plane), select a similar element on the 2^nd component, click on arrow to flip (or somewhere else to finish 1^st constraint), repeat to create 2^nd and 3^rd constraint (if more than one constraint is required for proper orientation).

Back to Adding non “rigged” Components

Back to Constraints Icon group (Assembly)

Moving/Copying a part to another sub-assembly

-Make sure that the part and assembly is in Design Mode.

Click (or right-click) on the Instance (in the Tree) to be copied, Copy (Ctrl-C), select the sub-assy (in the same Model Tree) that the part/component will be copied to, click (or right-click), Paste (Ctrl-V).  If you wanted to move instead of copy: right-click on the original, Delete; or just Cut (Ctrl-X) instead of Copy.  If you are Pasting (Ctrl-V) multiple copies you will have to select the copied Instances after each Paste.

-Review the conversation in Moving an instance with the Compass to consider your assembly choices.

Back to Creating a sub-assembly in an assembly

Back to Other moving with the Compass tips

Opening a part/component in it’s own window:

Double click on the component to make sure it’s activated, right click on the component, filename.1 object >, “Open in new window”.

Access the other in session models at the bottom of the Window pull-down menu.

Product Structure Tools icon group:

            Define Multi Instantiation (Patterning components)

            Fast Multi Instantiation

See Assemblies for applicable “Product Structure Tools” applications.

Define Multi Instantiation (Patterning components)

-If the part that the component will be interfacing with was Patterned (e.g. Rectangular Pattern) then use: Reuse Pattern instead since it keeps an associated link to the part’s pattern and will populate the part’s pattern (with the component) automatically.

-Before starting make sure that the desired assembly (that will be populated with the new copies) is highlighted blue (double click until it remains blue) and any components that will be selecting is in Design Mode.

Select the Define Multi Instantiation icon , enter the number of additional copies of the component in the “New instance(s)” field, enter the spacing between copies in the Spacing field, In the “Reference Direction” section define the move direction by selecting an existing edge, select the component to copy (this will populate the “Component to Instantiate” field), toggle the Reverse button until desired direction is found, keep the “Define As Defualt” radio button checked, press OK or Apply.

-If the same exact spacing is to be applied again use Fast Multi Instantiation which utilizes the last “Define Multi Instantiation”.

Back to Rectangular Pattern

Fast Multi Instantiation (uses the last “Define Multi Instantiation” settings [as long as the “Define As Defualt” radio button was selected]).

Select the Fast Multi Instantiation  icon, select the component to be patterned copied.  The selected component will be copied per the last Define Multi Instantiation definition.

Reordering (Graph Tree Reordering)

Select the Graph Tree Reordering  icon, enlarge the window by dragging the corners (if desired), highlight the component to be reordered, select the up or down arrow to move the component to the new location in the Tree.  Use the Graph Tree Reordering icon to order your components in alpha-numeric order.

Retrieving latest components (while they are in session):

If you added components from the server (files are in more than one directory) you can retrieve the most up to date versions by replacing them by the same procedure as in Repairing a component’s broken links.  This is helpful when other people are updating their files while you have their components in session.

Unload Components (Erases component from memory).

Right-click on component, Components, Unload

Sometimes the best way to Load the part back is to close down Catia and restart session.

See Repairing a component’s broken links to Load the part back (Links…Replace or Load).

Back to File, Save As

Broken links (Desk):

File, Desk: Black files are Unloaded; Red files weren’t found

-To leave the Desk: File, Close (or leave it open and access it from the Windows pull-down menu).

-Familiarize yourself with the right-click menus in Desk.  The menu includes the option to Open any model.

-Red components are components that can’t be found.  Hopefully you can avoid these red components (by using Save Management or Replace Component).  But if you do get a red component in Desk simply do the following: Right-click on these red components and select  Find, browse to the new location of the file.  Even if an error window pops up the component should become loaded (and turn white).  Save the assembly, close it and reopen to make sure there are no more disconnects (no more red components in Desk).

Note: To show latest information close (File, Close) the Desk and reopen.  To force a component to turn red (if you removed the part while the assy was in session): right-click, select Unload (the component should turn red).

See Links for more information.

Back to For view maintenance purposes:

Back to Rename

Back to Saving (Save As) many files

Drawings (a brief look)

            Intro to Drawings

            BOM

Drawing Format Help

Text & Callouts

Printing

Views (Drawing Views)

Assembly Constraints

Assembly Constraints Icon group

            Assembly Coincidence Constraint

                        Modifying Assembly Coincidence Constraint

            Reuse Pattern

-Review the conversation in Moving copied Instances with the Compass to consider your assembly choices.  Also review making Patterns in parts (e.g. Rectangular Pattern) since this can simplify assembly of many common components that interface with a patterned feature.  This simplified assembly is accomplished with the Reuse Pattern assembly constraint.

-Before initiating the “assembly constraints” the component’s parent assembly must be:

-highlighted blue

-The assembly requires at least one component

-Any components that you will be selecting must be in Design Mode and be a component that is indentured “under” the highlighted blue assembly.  If this restriction does not allow for ample references than use the Moving an instance with the Compass or Move Icon Group (Assembly) instead.

Note on highlighting the correct assembly:

While in an assembly, double click the assembly (to make highlighted blue) who’s next indentured components will be aligned with “assembly constraints”.  These top level sub-components (next indentured components) will move as a whole (i.e. lower level components move together with these parent “top level sub-components”) when constrained per the above assembly constraints.

-A  branch will be added to the assemblies Assembly Tree.  Expand it to keep track of the Constraints that you create as you create them.

-Recommended to use the Update  icon following each constraint definition to see the results of each constraint.  Press Undo (Ctrl-Z) if the Update made selection difficult during the next Constraint definition.  In such instances, it’s recommended to press Update either when your part is fully, or partially, constrained. 

-You can expand the  branch and update the newly added constraint by selecting Update from the right-click menu.  The constraint icon will have a little yellow squirrelly (e.g.  instead of ) if it needs updating.  Sometimes the Update icon will still be grayed out so you will have to force the constraint to update by double-clicking on it (then the Update icon should be colored and ready to use).

-Undo after an Update will only Undo the Update and not the last Constraint unless Undo was selected twice.  So feel free to use Update temporarily (i.e. Ctrl-Z afterwards).

-Make sure that the parts that you will be selecting are in Design Mode or else their entities won’t be useable for selection.  See Design & Visualization Mode.

-Consider using the Fix Component  constraint for one of your components before applying other assembly constraints.

Tips for moving the part with the Compass

Tips for moving the part with the Compass

Moving copied Instances with the Compass

            Measure in Compass Manipulation Window

            Other moving with the Compass tips

            Snap Automatically to Selected Objects (orienting the Compass tip)

Moving copied Instances with the Compass

-Consider using this Compass move technique after you’ve placed your first Instances (of the parts you wish to have multiple copies of) with Constraints (Constraints Icon group (Assembly)).  This Compass technique is helpful to move copied components (as described in Moving/Copying a part to another sub-assembly).  At the very least, use the Compass to move copied components so that they are no longer atop of themselves (making selection of their surfaces easier).  After moving the copied Instances (so they are no longer atop of themselves), you may consider continuing to use the Compass or you may decide to add another Constraint (see Constraints Icon group (Assembly)).

Back to Constraints Icon group (Assembly)

Measure in Compass Manipulation Window (helps populate the U, V and W fields, etc.)

There is also a Measure (Measure, Distance) available when you are using the Compass to move the copied Instances/components.  This is very powerful when used with Moving an instance with the Compass since it will populate the correct fields of the Compass so that you will only have to select the  arrow (as long as your selected order was in the form of: source then destination, else: the  arrow) for each field that the Measure has populated.  Regardless, if you pick the wrong arrow just correct by picking the opposite arrow.  Don’t feel that you have to keep reorienting the Compass, this Measure-Distance method will populate the correct fields regardless of Compass orientation.

Note: Turn the Snap Automatically to Selected Objects setting off while Measuring within the Compass.

Other moving with the Compass tips

-When you have a pattern (per say) of Instances already in place and would like to copy the common pattern to another location within your assembly, use “multiple select” (Ctrl key) to pick them all.  Use the same procedure (Moving an instance with the Compass) to move all the Instance copies at once.  Maximize the benefit of this technique by thinking ahead (e.g. have all [e.g. stackup] of the Instances in place at the first location before coping to new location).

Snap Automatically to Selected Objects:

If a part/component was made symmetric to one or more of its default datum planes, it’s often helpful to right-click on the Compass and select “Snap Automatically to Selected Objects”.  This is often helpful to orient the Compass about a part’s centerline, etc. and orient it correctly if you desire to rotate the component with the Compass.

-This setting snaps pretty well to the component’s internal coordinate system (intersection of its default datum planes) if the Compass was moved from its Reset position (immediately before placing on the component).  But if you keep moving it around, without resetting, it gives more emphasis to the component’s surfaces.  Knowing this, it is recommended to Reset the Compass (see Resetting the Compass) before attempting to select a component (if snapping to a part’s internal coordinate system is desired).

Turn this Snap setting off while using the Measure in Compass Manipulation Window.

Resetting the Compass

Drag the compass and release on top of the axis  found in the lower right of the graphics window.  Continue this until the Compass returns to its home position (top right of graphics window).

-See View Orientation for information regarding View Orientation controls and toggling between the Tree and your geometry.

Back to Snap Automatically to Selected Objects

The Compass

When you’re in a single part model: refer to the compass’ orientation to help appreciate the orientation of each of the default datum planes (found at the top of the Modeling Tree).  The compass’ orientation (in a single part model) will be consistent with the x-y-z orientation of the xy, yz & zx planes (of the part).