Chapter 3 Sketch Mode.

Chapter 3 Sketch Mode

DesignModeler Geometry Length Units DesignModeler Geometric Entities
Sketch Mode Contents DesignModeler Geometry Length Units DesignModeler Geometric Entities Sketch Mode New Plane Button New Sketch Button “From Face” Plane/Sketch The Sketch Mode GUI Planes and Sketches Plane Transforms Sketching Tools Sketching - Basic Shapes Sketch Details Sketch Constraints Sketch Dimensions Dimension Editing Workshop 3-1, Sketching Modifying Sketches Sketch Instance Geometry Interfaces Attaching to a CAD Session Importing CAD Files Positioning Imports Import Units Exporting a Model Body Attributes Workshop 3-2, 3D Geometry December 17, 2004 Inventory #002176 3-2

Sketch Mode DesignModeler Geometry
To study DesignModeler geometry we’ll focus on four fundamental areas: Sketch mode: Contains tools to create 2D geometric shapes as a prerequisite to 3D geometry creation or concept modeling. 3D Geometry: Geometry derived from sketch entities such as extrusions, revolves, surface models, etc. Geometry import: Geometry originating from a commercial CAD system. Typically imported into DM to allow modification for FE meshing. Concept modeling: These tools are used to create and modify line and surface bodies which can be used as the basis for FE beam and shell models. December 17, 2004 Inventory #002176 3-3

Sketch Mode Length Units
When a new DM session is started a dialog box allows selection of the desired length unit (can be set as default) December 17, 2004 Inventory #002176 3-4

Sketch Mode DesignModeler Geometric Entities
Points 2D Sketch Points 3D Vertices PF Points (Point Features): spot-welds point loads construction points Edges (Lines, Curves) 3D, and 2D Sketch Faces (Areas, Surfaces) Bodies (Volumes) Multiple bodies (not shown) S Please keep the following terms distinguished: - Face -- a topological entity (has an underlying geometry: surface) - Surface -- a geometric entity - Sheet -- a body consisting only of faces (in the DS/WBE this will be treated as a "Shell") Analogously: - Edge - Curve, line - Wire ("Beam") December 17, 2004 Inventory #002176 3-5

Sketch Mode Sketch Mode
DM sketches are created on planes. In a new DM session there are three default orthogonal planes in place at the global origin (XY, ZX, YZ). Users may create and position new planes as needed by defining origin and orientation or by using existing geometry as a reference. The process to begin sketching is twofold: Identify the plane upon which you wish to sketch. Create or identify the sketch which lies on the desired plane. Users may create as many planes as needed. Each plane may have multiple sketches associated with them. In the next few pages we’ll look at plane and sketch entity creation and tools to assist in sketching. December 17, 2004 Inventory #002176 3-6

GUI - Graphical User Interface New Plane Button
>New Plane creates a new plane: New plane object is placed in the Tree Six types of plane construction (Detail Pane): From Plane – new plane is based on another existing plane From Face – new plane is based on a face From Point and Edge – new plane is defined by a point and a straight line edge From Point and Normal – new plane is defined by a point while its normal is defined by an edge direction From Three Points – new plane is defined by three points From Coordinates – new plane is defined by typing in the coordinates of the origin and normal Sketches are then added to plane A sketch is utilized to create 3D geometry December 17, 2004 Inventory #002176 3-7

GUI - Graphical User Interface New Sketch Button
New Sketch : creates new sketch on the active plane. New sketches are placed in Tree beneath their associated Plane. Navigate sketches (make active) via the Tree or drop down list. Note: drop down list references sketches on currently active plane (see example below). Only XYPlane sketches displayed in drop down XYPlane is active December 17, 2004 Inventory #002176 3-8

GUI - Graphical User Interface “From Face” Plane/Sketch Shortcut
Shortcut to create a new “From Face” plane and sketch using existing geometry: Highlight desired surface to place new plane. Switch to the Sketch tab and begin sketching. New plane and sketch are automatically created! December 17, 2004 Inventory #002176 3-9

Sketch Mode The Sketch Mode GUI
In sketch mode the GUI presents sketching “toolboxes” to the left through a series of panels. Plane and sketch creation and management Draw Panel At the beginning of a new session the XY plane is displayed at the origin. ToolBox Panels December 17, 2004 Inventory #002176 3-10

Sketch Mode Planes and Sketches
The active plane is highlighted in the tree and shown in the drop down list. Active plane can be changed from either location. Clicking the “New Plane” button results in a plane being created. The same functionality and behavior applies to sketch creation and manipulation. Note that each sketch will be associated with a plane. December 17, 2004 Inventory #002176 3-11

Sketch Mode Planes and Sketch Details
The plane origin can be turned on/off. After setting plane details, the “Generate” button creates the new plane. Note: this step is not necessary for sketch creation. Can “Generate” with RMB The “Details” for each plane and sketch controls basic behavior. Triad Ruler The triad and display ruler can be turned on/off. December 17, 2004 Inventory #002176 3-12

Sketch Mode Plane Transforms
Up to 9 plane transformations are available. They can be applied quickly by choosing the desired transform through the RMB in the “Transform” field in the plane detail window. December 17, 2004 Inventory #002176 3-13

Sketch Mode Plane Transforms…
Once a transform is selected, additional properties may appear that will allow you to enter offset distances, rotation angles, rotation axes, etc. This transform requires both an offset and a rotation angle. PLANE4 To add an additional transform, set Additional Transform? to Yes. December 17, 2004 Inventory #002176 3-14

Sketch Mode Sketching Tools - Grid
The “Settings” panel allows a sketch grid to be defined and displayed (default = off). Snap feature applies to major and minor spacing. Major spacing (solid) Minor spacing (dashed) December 17, 2004 Inventory #002176 3-15

Sketch Mode Sketching Tools – Grid…
Grid Snaps per Minor allows snapping to points in between minor grid lines. This rectangle is snapped halfway between two minor grid lines. December 17, 2004 Inventory #002176 3-16

Sketch Mode Sketching Tools – Ruler
The Ruler tool allows you to get a quick sense of scale. December 17, 2004 Inventory #002176 3-17

Sketch Mode Sketching Tools – Auto Constraints
By default DM is in “auto-constraint” mode. Auto constraints allow new sketch entities to automatically snap to a location or orientation. The cursor indicates the kind of constraint that will be applied. Examples: (see documentation for complete list) Vertical and Horizontal constraints while sketching a line. Point constraint at beginning of line sketch. Coincident constraint at beginning of line sketch. December 17, 2004 Inventory #002176 3-18

Sketch Mode Sketching Tools – Tips
When creating or changing planes and sketches the “Look At” tool will immediately orient the display so that the plane, sketch or selected entity is normal to your view. Many operations either require or are more efficient via a right mouse click context menu from the graphics screen. Right mouse click “RMB” December 17, 2004 Inventory #002176 3-19

Sketch Mode Sketching Tools – Tips …
The Undo/Redo buttons are available in sketch mode only. Removes the last completed sketching operation. Multiple undo’s allowed. IMPORTANT: Each plane stores its own Undo “stack”. The “Back” operation (available via RMB) acts like a micro undo during sketching operations. Remember: only one sketch is active at any time! December 17, 2004 Inventory #002176 3-20

Sketch Mode Sketching Tools – Tips …
The GUI status bar contains instructions on completing each operation. Example: using the circle operation . . . Choose “Circle” Follow instructions in status bar: choose location for center point Follow instructions in status bar: drag and release for radius December 17, 2004 Inventory #002176 3-21

Sketch Mode Sketching – Basic Shapes
Once a plane and sketch have been specified you can begin creating new geometry from the “Draw” toolbox. Remember! Some operations will require a right click to complete! Example: to end a “spline” operation use the RMB to choose the desired option. December 17, 2004 Inventory #002176 3-22

Sketch Mode Sketch Details
Reference numbers for the entities in each sketch (lines, circles, polygons, etc.) can be viewed. Useful for parametric modeling discussed later. Can rename sketches from Detail pane. December 17, 2004 Inventory #002176 3-23

Sketch Mode Sketch Details …
Highlighting lines in the graphics screen (sketch mode only), will display details for the line. Can rename sketch entities from Detail pane. Details for highlighted line December 17, 2004 Inventory #002176 3-24

Sketch Mode Sketch Constraints
Sketch details can also display sketch constraint details. Constraints may result from auto-constraints or user defined. To delete constraints, highlight the definition and use the delete key. Show constraints Constraint definitions December 17, 2004 Inventory #002176 3-25

Sketch Mode Sketch Constraints . . .
Sketch entities are also color coded to indicate their current constraint status: Teal: Under-constrained Blue: Well Defined Black: Fixed Red: Over-Constrained Gray: Inconsistent or Unknown Example: Initially sketched lines are displayed in teal color to indicate under-constraint. Note even when dimensioned, these lines are underconstrained since they are not fixed in space Adding 2 more dimensions resolves the sketch status and all lines are displayed in blue Teal Blue December 17, 2004 Inventory #002176 3-26

By adding too many dimensions and/or constraints the sketch will become over constrained. Over constrained lines are displayed in red in sketch mode Applying “Fixed” constraints to 2 of the edges shown here results in the lines being displayed in black Red Blue Red Teal Black December 17, 2004 Inventory #002176 3-27

The picture below demonstrates an inconsistent situation (lines displayed in gray). Here the arc is dimensioned with a radius of 5 however the vertical dimension has been specified as Obviously there is no way to maintain the connection between the 2 horizontal lines and the arc while maintaining these dimensions. Gray December 17, 2004 Inventory #002176 3-28

Sketch Mode Sketch Dimensions
DesignModeler contains a complete dimensioning toolbox. In addition to individual dimension assignment, semi-automatic dimensioning is available. Semi-automatic cycles through dimension choices until model is fully constrained or user chooses to exit semi-automatic mode. Right mouse button controls skip or end functions. The General dimensioning tool allows quick access to all primary dimensions via a right click context menu. Right Mouse Click December 17, 2004 Inventory #002176 3-29

Sketch Mode Sketch Dimensions …
Move function allows placement of dimension to be modified. Animate to view dynamic changes applied to the selected dimension. Dimensions can be displayed as the dimension value or name. December 17, 2004 Inventory #002176 3-30

Sketch Mode Sketch Dimensions …
To modify dimensions highlight then change value in details window. Highlight dimension Enter new value December 17, 2004 Inventory #002176 3-31

Sketch Mode Dimension Editing
Once highlighted, dimension can also be quickly edited through a RMB menu option, >Edit Name/Value. Note: a recent “Generate” might be necessary to see “Value” as well as “Name” December 17, 2004 Inventory #002176 3-32

Workshop 3-1, Sketching Using a simple example, let’s see how we put to use what we’ve seen so far (note RMB = Right Mouse Button). Goal: Sketch a rectangle 50mm high and 75mm wide with the bottom left corner at the origin. Add a 10mm radius circle within the rectangle with the center 20mm from the left side and 30mm from the bottom. Place all dimensions where they can be easily viewed. R = 10mm 50mm 75mm 30mm 20mm December 17, 2004 Inventory #002176 3-33

Workshop 3-1, Sketching >File>New, or Start DesignModeler (Geometry) stand alone mode When prompted, set length unit to millimeters December 17, 2004 Inventory #002176 3-34

Workshop 3-1, Sketching Icon When DM starts, switch to sketch mode using the sketch tab. Note: use the “Look At” icon (or RMB options) to orient the sketch plane in the normal direction. Select the “Rectangle” tool and place the cursor at the origin. Once the “P” (point constraint) symbol shows, click, hold and drag, then release to create the rectangle. RMB Click Drag December 17, 2004 Inventory #002176 3-35

Workshop 3-1, Sketching Icon Before continuing, click the “Fit” icon (or RMB menu). Now choose the “Circle” tool and click, drag and release to create a circle in the approximate location within the rectangle. RMB December 17, 2004 Inventory #002176 3-36

Workshop 3-1, Sketching We’ll now formalize the sketch by adding dimensions. Select the Dimension toolbox and leave the default selection at “General”. Click on the top line of the rectangle to display the proposed dimension. Place the dimension above the rectangle by dragging and clicking. December 17, 2004 Inventory #002176 3-37

Workshop 3-1, Sketching Repeat the preceding steps to add the remaining dimensions. Next modify the details for each dimension to the desired values as shown. 50mm D = 20mm 75mm 30mm 20mm December 17, 2004 Inventory #002176 3-38

Workshop 3-1, Sketching To complete our sketch use the “Move” function in the Dimension toolbox to position (drag) the dimensions (like below for example). December 17, 2004 Inventory #002176 3-39

Workshop 3-1, Sketching Now try animating several dimensions:
Choose the “Animate” function then click on a dimension in the graphics window. Change the dimension display from “Name” to “Value”. December 17, 2004 Inventory #002176 3-40

Workshop 3-1, Sketching As a last check of our stated goals go to the details for sketch 1 and change “Show Constraints?” to “>Yes”. Scroll down to the details for Line7 and note the base point is coincident with the origin - - DM captured our design intent during sketching. Note: leave DM session running as we will continue with this geometry later. December 17, 2004 Inventory #002176 3-41

Sketch Mode Modifying Sketches
The Modify toolbox contains a number of functions for editing sketches. Some functions are self explanatory (e.g. fillet, chamfer). This section will focus on some of the less obvious functions. Remember! - check the status bar at the bottom of the GUI for real-time instructions for each function. Status Bar - Example December 17, 2004 Inventory #002176 3-42

Sketch Mode Modifying Sketches …
Split: RMB Options (choose before selecting edge): Split Edge at Selection (default): splits an edge into two pieces at the selection location (unless the edge is a full circle or ellipse). For a full circle or ellipse, both start and end endpoints are created at the selection location. Split Edges at Point: Select a point, and all edges, which pass through the selected point, are split there. Split Edge at All Points: Select an edge and it is split at all points that it passes through and that have a coincident constraint to it. Split Edge into n Equal Segments: Set the value n in the edit box and then select the edge which you want to Split. Note: up to 100 allowed for n. “Split” is useful for sketches to be used with Skin/Loft “Split” edges also offer greater control in subsequent meshing and/or boundary condition operations. December 17, 2004 Inventory #002176 3-43

Drag: Can drag a point or edge using the cursor. How the model changes depends on what is selected, existing constraints and dimensions. Can pre-select multiple entities before issuing the Drag function. Drag - Example Select corner point of rectangle and drag. Drag December 17, 2004 Inventory #002176 3-44

Cut/Copy: Requires the selection of a paste handle (RMB) relative to which the Paste will be performed. The paste handle is the location to which the cursor is attached while you are moving the image into position to paste. RMB paste handle options: End / Set Paste Handle, and specify the paste handle. End / Use Plane Origin as Handle, the 0.0, 0.0 location of the plane will be used as the paste handle End / Use Default Paste Handle, the start of the first curve selected will be used as the handle This lets you select a set of items to copy to an internal clipboard, and leaves the originals in the sketch. If Cut or Copy is exited without selecting a paste handle, a default will be used. Copy: RMB options. December 17, 2004 Inventory #002176 3-45

Paste: RMB Context Menu: Rotate by +/- r Degrees Flip Horizontally / Vertically Scale by Factor f or 1/f Paste at Plane Origin Change Paste Handle End Paste lets you take items placed on the clipboard by Cut or Copy and place them into the current (or new) sketch, even if it is on a different plane. December 17, 2004 Inventory #002176 3-46

A Copy/Paste example . . . After creating a rectangle we wish to copy it, rotate it by 45 degrees with respect to the origin and scale it by a factor of 0.5. RMB Copy Select edges December 17, 2004 Inventory #002176 3-47

RMB Rotate RMB Scale Choose Paste and set options RMB Paste RMB End Notes on Copy/Cut/Paste: After copying, paste can be done multiple times. Can copy from one sketch and paste to another. During Paste operation you can change the paste handle. December 17, 2004 Inventory #002176 3-48

Sketch Mode Modifying Sketches – Quick Cut/Copy/Paste
Cut, Copy, and Paste commands are available as RMB options in sketching mode. 1) Select source edges 2) RMB>Copy 3) Select paste origin 4) Paste the edges December 17, 2004 Inventory #002176 3-49

Replicate: The Replicate command is equivalent to the Copy command, followed by a Paste. After one of the End / options is selected, the right mouse button changes to the Paste right mouse button. Move: The Move command functions the same as the Replicate command with the exception that your original selection is moved to a new location instead of being copied. December 17, 2004 Inventory #002176 3-50

Offset: The Offset function allows you to create a set of lines and arcs that are offset by an equal distance from an existing set of lines and arcs. The original set of lines and arcs must be connected in an open or closed profile. Preselect or select the edges then choose the right mouse button option “End selection / Place offset” The cursor location is used to determine three things: Offset distance Offset side Offset area Distance and Side are clear but the “area” is very important: If portions of your selected curves would collapse out or cross over one another given the current offset side and distance, the cursor location determines which area of offset curves is kept. An example . . . December 17, 2004 Inventory #002176 3-51

First we choose all edges to be offset The direction and distance the cursor is moved determines the offset. December 17, 2004 Inventory #002176 3-52

Notice as the offset is dragged further, the arc will eventually intersect the bottom line. By alternating the cursor location (left and right) we can determine which offset region will be retained. December 17, 2004 Inventory #002176 3-53

Sketch Mode Sketch Instance
Sketch Instancing allows copies of sketches to be added in other planes. The copies are persistent, meaning they will update when the source sketch is updated. Features: Edges in a sketch instance are fixed (like a plane boundary) and cannot be moved, edited, or deleted by sketch operations When changes are made in the base sketch its instances will be updated when a Generate is done A sketch instance can be used just like normal sketches for creating other features except: Cannot be used as base sketches for other Instances Sketch instances are not included in the pull-down list of sketches Step 1: Choose the destination plane for the instance. The source sketch must be in a plane prior to the destination plane (higher in Tree). Therefore, you can never place a sketch instance onto the XYPlane. December 17, 2004 Inventory #002176 3-54

Sketch Mode Sketch Instance…
Step 2: Choose the source sketch via Apply/Cancel buttons. Step 3: Modify the placement options. The sketch instance may be offset, rotated, and scaled. Step 4: Click Generate to complete the sketch instance. December 17, 2004 Inventory #002176 3-55

Sketch Mode Sketch Instance…
Example: Sketch2 is instanced onto Plane4 as Sketch5. Note how the instance appears as fixed edges, similar to plane boundary edges. December 17, 2004 Inventory #002176 3-56

Geometry Geometry Interfaces
DM >File>Import & >File>Attach capability: Can Import/Attach anytime, even multiple times per model Can add, subtract, etc. during Import/Attach process Base Plane Property for orientation The following CAD versions are supported: ACIS BladeGen – (DM-CFX Course) Parasolid - 16 SolidWorks SP4 / 2004 Solid Edge - V15 / V16 Mechanical Desktop – 2004DX /2005 Autodesk Inventor – R8 / R9 Unigraphics – NX 2.0 / NX 1.0 CATIA - V4 CATIA - V5 (R2 - R13) Pro/ENGINEER – 2001 / Wildfire 1 & 2 IGES Reader - 4.0, 5.2, 5.3 December 17, 2004 Inventory #002176 3-57

Geometry Attaching to a CAD Session
If a CAD session is currently open, this automatically imports the model into the DesignModeler session File>Attach to Active CAD File Maintains bi-directional associativity December 17, 2004 Inventory #002176 3-58

Geometry Importing CAD Files
File>Import External Geometry File… The “active” plane controls placement for “assembly” modeling (multi-bodies). The details pane import type: Add, Cut, Slice, etc… Does not maintain associativity Active Plane Add Cut December 17, 2004 Inventory #002176 3-59

Geometry Positioning Imports
Both Import and Attach have a “Base Plane” property. Specify the plane (orientation) in which the Import or Attach model is referenced… When creating a new Import or Attach feature, the active plane is chosen as the Base Plane by default Users select planes from the tree view or Plane pull-down list prior to import Example: XY chosen for first import YZ plane for second import Add material option chosen The Base Plane for Imports and Attaches in all agdb files prior to this upgrade is XYPLANE December 17, 2004 Inventory #002176 3-60

Set the desired length unit when DM starts
Geometry Import Units Set the desired length unit when DM starts Some import types allow you to set the units via the import details (Prior to Generate) DM then converts the model length units into the current unit system December 17, 2004 Inventory #002176 3-61

Geometry Exporting a Model
File>Export … IGES exporting: When exporting the model to an IGES file, you have the option to export solids or just trimmed surfaces. >Tools>Options December 17, 2004 Inventory #002176 3-62

Geometry Body Attributes
DM supports two kinds of body attributes through Import and Attach features : Surface body thickness Material properties Material properties are controlled by the Import Material Properties option in the property list for Import and Attach features. If set to >Yes, then any material properties will be processed with the bodies. Material properties are read-only in DM – they are brought in through the Import and Attach features, but you cannot edit them. Properties are transferred with the model when sent to Sim. December 17, 2004 Inventory #002176 3-63

Geometry Body Attributes…
Surface body thickness is transferred to DM from CAD systems that support it. Users can modify the thickness of any surface body in DM. The thickness will be attached to the surface bodies when the model is sent to Sim. December 17, 2004 Inventory #002176 3-64

Workshop 3-2, 3D Geometry Goals:
Utilize the model created in Workshop 3-1 and generate 3D geometry from the sketch. Create a new sketch and extrude it to create a boss on the original model. Create another sketch and Imprint a face on the boss to allow for applying boundary conditions to an FE model. Save the model and Exit. Start Page (if workshop 3-1 was closed): Choose the option “Open” December 17, 2004 Inventory #002176 3-65

Workshop 3-2, 3D Geometry Continue with the database created in Workshop 3-1 If this is not available open the file called “Workshop 3-1.agdb” and continue with workshop 3-2. With the model open choose the “Extrude” icon from the toolbar. In the extrusion details change the depth to 10mm. Generate the extrusion. 1 3 2 December 17, 2004 Inventory #002176 3-66

Workshop 3-2, 3D Geometry Insure that the XYPlane is active and click on the “New Plane” icon. In the Details of Plane4 set Transform 1 to be “Offset Z” and change the offset “Value” to 50mm. “Generate” the Plane. 4 6 5 December 17, 2004 Inventory #002176 3-67

Workshop 3-2, 3D Geometry Click the “Look At” icon to reorient the view. Switch to Sketching mode and choose “Rectangle” from the drawing toolbox (check Auto-Fillet box). [Sketching] >Draw>Rectangle Draw a rectangle and utilize Auto-Fillet approximately as shown here. Click on the “Dimensions” toolbox. [Sketching] >Dimension 7 9 10 8 December 17, 2004 Inventory #002176 3-68

Workshop 3-2, 3D Geometry Dimension the sketch as shown below Note: your dimension names may not match those shown. 11 11 December 17, 2004 Inventory #002176 3-69

Workshop 3-2, 3D Geometry From the toolbar choose “Extrude” (do not generate yet!). An isometric view shows the proposed (wireframe) extrude using a surface- normal direction (facing away from the original model). From the Detail window change the direction field from Normal to “Reversed”. Change the Type to “To Next” “Generate” the extrusion. 15 12 13 14 December 17, 2004 Inventory #002176 3-70

Click on >Display Plane button to turn off plane
Workshop 3-2, 3D Geometry The extrude operation creates the boss which is merged with the original geometry. Click on >Display Plane button to turn off plane + dimensions if necessary December 17, 2004 Inventory #002176 3-71

Workshop 3-2, 3D Geometry 18 17 In our FE simulation we wish to add a boundary condition at an arbitrary location on the boss. We will imprint a face on the boss for that purpose. Select (Highlight) the top surface of the boss. Click the “New Plane” icon in the toolbar. “Generate” the plane. 16 December 17, 2004 Inventory #002176 3-72

Workshop 3-2, 3D Geometry Click the “Look At” icon from the toolbar.
Go to sketch mode and choose circle from the draw toolbox. [Sketching] >Draw>Circle Draw a circle approximately like the one shown here. 19 20 21 December 17, 2004 Inventory #002176 3-73

Workshop 3-2, 3D Geometry Add dimensions as shown at right. Note your dimension names may not match those shown here. [Sketching] >Dimensions>General 22 December 17, 2004 Inventory #002176 3-74

Workshop 3-2, 3D Geometry Choose “Extrude” from the toolbar (do not Generate). In the details change the operation to “Imprint Faces”. “Generate” the extrusion 25 23 24 December 17, 2004 Inventory #002176 3-75

Workshop 3-2, 3D Geometry Make sure the surface selection filter is active and highlight (select) the circular surface on the boss. (Rotate the Model as Desired) Notice we now have a circular area that we can use for localized boundary conditions in our simulation. Exit without saving: “File>Exit Workbench” December 17, 2004 Inventory #002176 3-76

Chapter 3 Sketch Mode.

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Chapter 3 Sketch Mode.

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