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Solid Edge Tips and Tricks

Tushar Suradkar
www.oocities.org/SeGuruCool

  segurucool @ indiatimes.com


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      General Tip : Soothing Background new  

    Added : 09 April 2005

    This is not a trick - just a tip (comments invited)

    Graded backgrounds for eg. "Top-White (255 255 255) => Bottom-Light Blue (0 0 255)" are "biologically" correct since they resemble the horizon.

    It seems to calm down the brain somehow.

    In Solid Egde, select Format > View > Backgroung Tab > Type:Gradient > Select1 > More > Define Custom Color.

    Use the above RGB values.

      Draft Tip : Super Fill new  

    Added : 31 Mar 2005

    Did you know - you can copy a fill by drag-droping it from one area to another with the Ctrl key pressed,

    The fill gets copied and automatically conforms to the new shape.


      Draft Tip : Text Along a Curve new  

    Added : 22 Mar 2005

    You can have text along a curve in Solid Edge Draft too.

    The trick here is to create it in the Part environment and simply copy-paste it in a Draft sheet.

    Whats more ! you can even edit it by double clicking right inside the draft environment.

    Note : Creating text along curve is now available in the Draft environment in Solid Edge 17.

    Read whats new in Solid Edge 17 - Here.

      Draft Tip : Non Rectangular Crop new  

    Added : 12 Feb 2005

    You can crop a view in a non-rectangular fashion also.

    The trick here is to create a detail view.

    When creating the detail view, click the Define Profile button on the ribbon bar.

    Next Keep the scale of the detail view to 1 and effectively you have a non-rectangular cropped view.

      Assembly Tip : Rotate Preview and Drop new  

    Added : 19 Jan 2005

    You can drop a part in an assembly in an orientation diferent from when it was created.

    In the Preview window in the Edgebar, use usual mouse keyboard-controls to rotate the part and have the desired face/edge visible.

    Drop the part now and expect it to appear in the assembly in a new orientation as in the preview.

      Sheetmetal Tip - Double Dimple new  

    Added : 21 Dec 2004

    You can trick Solid Edge into creating a nested dimple by setting the radius to zero for the first dimple.

    Read an indepth tutorial on how to do this.

      Drafting Tip - Quick Quicker Quickest new  

    Added : 12 Sept 2004

    The QuickPick prompt can dig deeper than you may think.

    Ever ungrouped a group and grouped it back just to edit an entity inside it.

    Using the QuickPick prompt, you can do this without having to ungroup the group.

    See figure.

    A tiny utility to do this via a sleek dialog interface is here.
    This utility can be used to edit Attribute data from a AutoCAD file opened in Solid Edge.

    Modeling Tip - Rotate features new  

    Added : 24 Aug 2004

    By pressing the n key at the keyboard, you can paste a copied feature in a rotated position.

    This saves you the hassle of later rotating the profile manually. See figure.

    Dimensioning Tip - Multiple Lines new  

    Added : 17 Aug 2004

    You can create multiple lines of text for a dimension Subfix.

    Select a dimension and click the Prefix tool on the ribbon bar.

    In the Subfix combo box, press Shift+Enter to add multiple lines of text.

    A vertical pipe | symbol seperates the multiple lines.

    See figure.

      Drafting Tip - Unlimited Jogs

    Added : 04 Aug 2004

    You can create multiple break lines for most annotation objects like the Callout, Leader, Feature Control Frame, etc.

    To do this, select the annotation object and then click it again with the Alt key pressed.

    This creates an extra handle, which you can drag as required (see figure). Repeat this as many times.

    To remove any of the handles, just Alt + Click on the handle.

    Using the same technique, you can also create Jogs for a Coordinate Dimension.

    An extra benefit with the Coordinate Dimension is that it has a Remove All Jogs tool on the ribbon bar.

      Sketcher Tip - DOF Colors

    Added : 26 July 2004

    Solid Edge allows you to display the color for an element based on the degrees of freedom (DOF) for the element.

    For example, an element that is fully defined (constrained) displays in a different color than an element that is not fully constrained.

    To specify the colors, select Tools > Options... and take the Colors tab.

    To use the color scheme, select Inspect > Sketch Relationship Colors.


      Assembly Tip - Insert Without Rels

    Added : 19 July 2004

    You can keep the Shift key pressed when dropping a part from the Edgebar into an assembly.

    This places the part without adding a single assembly relationship.

    The advantage of doing this is, you can first move and/or rotate the part in a near-to-final position for better vizualization before you start applying assembly relationships.

      Drafting Tip - Super Quick Views

    Added : 14 July 2004

    You can quickly create drawing views bypassing the Drawing View Wizard.

    Drag and Drop a Solid Edge document from Windows Explorer or the Library tab of the Edgebar directly on to a drawing sheet.

    Views will be created as follows :

  • For assembly models, an isometric view is created.

  • For all other models, top, front and right views are created.


  • Note : If you keep Shift pressed, the Drawing View Wizard will appear.

      Toolbar Tip - Shell Applications

    Added : 7 July 2004

    Ever wanted to quickly calculate and found yourself wading up-and-down all the menus through Start > Programs > Accessories >

    Ever wanted to have a special character in a textbox or callout.

    Launching an external application from right inside Solid Edge is as easy as 1-2-3...

    Right-click on any toolbar in Solid Edge and select Toolbars... or select View > Toolbars...

    In the Toolbars dialog, click New and type in the name for the new toolbar, something like Shell Applications or may be your pet's name will also be ok.

    A new toolless toolbar will appear somewhere on your screen, usually in the top-left corner of the Solid Edge window.

    Also, the Toolbars dialog will excuse itself and a new Customize dialog will appear.

    Scroll the categories list-box and select Macros from the list.

    In the Macros area on the right side, click the Browse... button.

    Now you can select a folder where any application of your choice sits.

    For Calculator and Character Map, browse to the C:\WINNT\system32 folder.
    I can say this folder for sure since Solid Edge, begining V14 supports Win2k and not Win98 anymore.

    Anyway, now you should have all files with a dll or exe extensions in the right-side list.

    Select charmap.exe for Character Map (or calc.exe for Windows Calculator)

    Drag and drop charmap.exe from the list onto the nascent toolbar.

    This brings up the Custom Button dialog, where you can select from 18 pics that Solid Edge provides so generously.

    Alternately, you may click the Browse... button in the Custom button dialog to select an existing 16x16 sized bmp file.

    Remember your program will launch even with a blank icon.

    Click Assign... then Close on the Customize dialog and you are done.

    Repeat the steps to add more tools.

      Sketcher Tip - Quick Connect

    Added : 30 June 2004

    Ever spent time sketching a complex profile only to get a warning on Finish that few of elements are not connected.

    Ever spent more time using the Connect geometric relationship to fix everything.

    Here's a quick way to do that...

    Click the Trim Corner tool
    and drag the mouse over the two entities you want to Connect.

    This will automatically place the connect relationship which was lost earlier, saving you many clicks and time.

      Dimensioning Tip - Single and Double Click  

    Added : 21 June 2004

    The dimension value textbox on the ribbon bar is capable of accepting much more than simple numeric values.

    When you single click on a dimension in the sketcher, you can enter mathematical expressions including parentheses.

    For example, 30+(7/4) and Solid Edge evaluates and assigns it to the dimension value.

    On the other hand, when you double-click on a dimension value, you have a formula strip on the ribbon bar.

    Here, you can include more advanced mathematical functions like LOG, ABS, FIX, INT, etc. and trignometric functions like SIN, COS, etc.

    The best part is, you can reference other dimensions like in MS Excel.

    For example, as shown in figure, say you want the length (horiz. dimension) of the rectangle to be always 1.5 times its height (vert. dimension).

    Here, double-click the length dimension to get the formula strip on the ribbon bar.

    Next single-click the height dimension for the rectangle upon which its name (reference) will appear in the formula strip. (see figure)

    Now simply add * 1.5 to it and press <Enter> at the keyboard and you are done.

    The length now automatically is a driven dimension of the height.

      Sketcher Tip - Window and Crossing

    Added : 14 June 2004

    This tip is for AutoCAD users who have recently upgraded to Solid Edge.

    In AutoCAD, if you have used the window(w) and the crossing(c) option of object selection, they are readily present in Solid Edge too.

    In Solid Edge, when selecting entities, take the Inside option on the ribbon bar. This is the equivalent of Window(w) in AutoCAD.

    Just next to this is the Overlapping option on the ribbon bar, which is the equivalent of Crossing(c) in AutoCAD.

      Sketcher Tip - Smart Angular Dimensions

    Added : 7 June 2004

    You can place an angular dimension for a line in four possible place using just the Smart Dimension tool.

    Start the command and select a line.

    Just before you place the dimension, hit the a key on the keyboard.

    Now you are placing an angular dimension without the need for an extra reference line.

    Move the mouse cursor into different intent zones to have four possible placement options as shown in figure.

      Drafting Tip - NonCircular Detail View

    Added : 1 June 2004

    Begining V15, you can make non-circular detail views too.

    After you click the Detail View tool, select the Define Profile option on the ribbon bar.

    This takes you to the sketcher mode, where you can draw a closed profile of any shape.

    Click Finish when done.

    Now you can proceed to create a detail view.

      Drafting Tip - OLE with Borders

    Added : 24 May 2004

    You can have OLE objects inserted in a draft sheet with or without borders, automatically.

    To insert OLE objects with a border, select Insert > Object... and browse to the desired file.

    To insert OLE objects without a border, drag and drop the desired file directly from Windows Explorer onto the draft sheet in Solid Edge.

    And irrespective of the method used, you can always toggle the border display by right-clicking on the OLE object and selecting Properties from the menu.

      Drafting Tip - Exporting to DWG with Automatic Layers.

    Added : 17 May 2004

    You can have layers generated automatically When exporting a Solid Edge draft file as AutoCAD drawing,

    To do this, open the SEACAD.ini that sits in the Program folder of Solid Edge and change settings to match as shown below. :
     
    Part Layers = 1
    Export Drawing View To Block = 0
     
    For an assembly view, layer names will be generated from part file names and all occurrences of a part will be placed on the same layer.

    Similarly, for a part views, layer names will be generated from part names and all views of a part will be placed on a single layer.

    Note : Do not modify the original SEACAD.ini file, but make a copy of it.

    In Solid Edge, click the options button in the Save As dialog box and specify the new ini file in the AutoCAD Translation Wizard.

      Sketcher Tip - Easy Polygons

    Added : 10 May 2004

    Even though Solid Edge lacks a generic polygon tool, its extremely easy to make one.

    Begin with a creating a circle and toggle it to Construction.

    Using lines, create an irregular polygon inscribed in the circle. (see figure)

    Using the equal geometric relationship, make the first line of the irregular polygon equal to the second line.

    Similarly make the second line equal to the third and so on.

    Finally make one of the lines horizontal using the Horizontal/Vertical relationship.

    The dimension of the circle will control the size of the polygon whose sides can number begining three and above.

      Sketcher Tip - SmartDimension

    Added : 3 May 2004

    The SmartDimension tool in Solid Edge sketcher is smarter than you may think.

    You can save extra clicks requred to dimension an inclined line that are required when using the Distance Between tool.

    Begin dimensioning an inclined line using the Smart Dimension tool (see figure)

    After selecting the inclined line, keep the Shift key pressed and move the mouse.

    Now you can apply horizontal or vertical dimension too (see figure)

    Release the Shift key and you are back dimensioning the inclined line.

      Sketcher Tip - Making base feature symmetric

    Added : 27 April 2004

    In Solid Edge, making a base part symmetric about the two reference planes is not only a good practice but also extremely easy.

    A quick way to do this is by using the Horizontal/Vertical constraint.

    Simply pick the midpoint of a vertical line (see figure)

    Then pick the endpoint of the horizontal reference plane. (see figure)

    Similarly, do this for the horizontal edge.

    This makes the base feature symmetric about the two reference planes.

      Modeling Tip - Apply larger rounds first

    Added : 20 April 2004

    The case is you want to create the rounds as shown in figure.

    You start with an object as shown.

    Suppose you apply the small round first.

    And then the larger round,
    not only, Solid Edge senses that it as a feature with problems, but

    the result is also not the desired one.

    You can rectify this problem by dragging and dropping the last round feature before the previous one in the feature pathfinder.

    This is also called feature re-ordering.

    Even if, feature reordering is a handy tool, apply larger rounds first.

      Modeling Tip - Keep rounds at the last

    Added : 12 April 2004

    The case is you want to give draft to a face that has rounded edges along the directions of the draft.

    See figure.

    Suppose you apply the rounds first.

    Ans then apply the draft -

    the feature won't fail but the result won't be desirable.

    Whether its a draft or any other feature, always keep rounds as the last feature.

      Drafting Tip - Exporting to DWG with Intelligent Dimensions.

    Added : 5 April 2004

    When exporting a Solid Edge draft file as AutoCAD drawing, dimensions in Solid Edge are converted to blocks in AutoCAD.

    Even after exploding the blocks in AutoCAD, you cannot edit them as dimensions.

    At most the text can be modified using the ed command or Ctrl + 1

    To convert as dimensions in AutoCAD, open the SEACAD.ini that sits in the Program folder of Solid Edge and change settings to match as shown below. :
     
    Break Dimensions = 0
    Stroke Dimension = 0
    Export Drawing View To Block = 0
     
    Note : Do not modify the original SEACAD.ini file, but make a copy of it.

    In Solid Edge, click the options button in the Save As dialog box and specify the new ini file in the AutoCAD Translation Wizard.

      Modeling Tip - Prefer cutouts to holes

    Added : 28 March 2004

    Whenever possible and if the design allows, use cutout instead of the hole feature.

    Using cutouts instead of holes reduces the file size.

    Especially when you have large number of holes (for e.g. 12 flange couplings with 12 holes on each flange (total 288 holes/cutouts).

    See for yourself :

    Flange-Holes.par = 221.50 kb (226,816 bytes)

    Flange-Cutouts.par = 206.50 kb (211,456 bytes)

    Download Solid Edge 14 zipped files (150 kb)

      Productivity Tip - Use Toolbars : not Dialogs.

    Added : 21 March 2004

    When hiding/showing reference planes, sketches, curves, axes, etc in Solid Edge, it becomes very cumbersome and time consuming to click on the Construction Display     tool every time and then clicking buttons and then clicking OK.

    Thats lot of clicking !

    You can easily create a toolbar called On/Off and include the various tools on it.

    The tricky part is that the various on/off tools found together in the construction display dialog are scattered under different Categories in the Customize Toolbar dialog.

    This tip shows you which Category to look for in the Customize Toolbar Dialog :

    Tool Category
    Reference Planes   Reference
    Reference Axes   Reference
    Sketches   Sketch
    Surfaces   Surfacing
    Curves   Surfacing
    Design Body   Model

    And although the toolbra may occupy some space on the screen, it is far more convinient to quickly make the object display On/Off with minimum number of clicks.
    Tushar Suradkar     segurucool @ indiatimes.com

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