Friday, December 18, 2015

Insert Assembly Copy

Solid Edge has had the command Insert Part Copy for a long time.  Insert Part Copy functions by allowing you to insert the geometric body of an existing Part, Sheet Metal or Assembly file into another Part or Sheet Metal file.  The geometric body can be optionally inserted associatively as an Ordered feature, or non-associatively in Synchronous mode and supports several options such as making the body a construction, scaling, or mirroring the inserted body.


A similar command was made available in ST5 and later versions called Insert Assembly Copy.  Insert Assembly Copy functions by allowing you to insert an existing Assembly file into another Assembly file.  Unlike Insert Part Copy which inserts a body, Insert Assembly Copy inserts the actual assembly structure under an Assembly Copy node in Pathfinder.  The resulting Assembly Copy is associative to the original such that any changes or additions to the original will be reflected in the copy.   You can of course freeze or break the link of the Assembly Copy which results in the Assembly Copy node becoming non-associative to the original.



The Insert Assembly Copy command has several options which are:
  • Add new components on update (If this is unchecked, adding new parts in the copied from assembly does not update the Assembly Copy with the new parts)
  • Include assembly features
  • Mirror about (uses the same wizard as the Mirror Components command)
  • Exclude Components



Uses for the Insert Assembly Copy include:
  • Creating a mirrored assembly (Left Hand vs. Right Hand)
  • Inserting a base 80% assembly into multiple assembly files and adding optional parts in each to produce 100% configured assemblies.
  • ???  If you can think of any other novel uses, please comment them on this article.

The Assembly Copy function is also used by:
  • The Mirror Components command in Assembly to associatively mirror assembly structure/components.
  • The Multi-Body Publish command to build an assembly of the published bodies for downstream use.

Wednesday, December 09, 2015

Solid Edge Wins Big at the “Slots”!



Solid Edge ST5 introduced a new “Slot” feature to make creating slots much more efficient than past methods.  You may have overlooked this feature in ST5 and future versions due to its nested button location on the ribbon, so I thought I would reintroduce this useful feature.

Prior to the new Slot feature, one would have to use the Cutout command and then create a sketch of the slot’s profile by hand or by using the Symmetric Offset sketch command.  If the slot needed to be counter bored for a head of a fastener, then additional sketching and features were needed.  The new Slot command simplifies this process greatly.

The Slot command is located under the Hole fly-out menu.  It is available as both an Ordered and Synchronous feature.

Invoking the command produces the Slot Command Bar that contains the typical command steps and option button that we are familiar with from other features (Ordered shown).

The Option button produces the standard Option form allowing us to set the active feature options as well as save them for later use.  The Slot command has the following options:

  •  Slot Width
  • Flat or Arc end
  • Counter bore/boss and corresponding offsets

The only sketch input needed for the slot is an open path for it to follow, which also defines its length (width is defined in the Options).  Tangent connected lines and arcs are supported.  As typical to sketch based features in Ordered, the sketch may be pre-created as a standalone Sketch feature or created during the Slot feature.  As typical in Synchronous, the sketch must be pre-created as a Sketch.

Monday, November 09, 2015

Dimension Projection Line Breaks

Often when placing dimensions on drawings, the projection lines of some dimensions will cross the projection lines of other dimensions as shown below.

Solid Edge provides a function to automatically create breaks in one extension line where it crosses another. This function is called "Add Projection Line Break". It is accessible from the Shortcut Menu when you have a dimension highlighted.




The result is shown below.


If you wish to remove the projection line break, highlight the dimension, invoke the shortcut menu, and select "Remove Projection Line Break".

Thursday, August 21, 2014

That One Thing in Solid Edge ST7…

Whenever a new version of Solid Edge is released, there is always a multitude of new/enhanced features and I’m usually asked by someone what my favorite one is.  You cannot imagine how hard that is to answer when your looking at hundreds of potential favorites in a given release.  Usually though, I find that it is the simple little things that seem to be my favorite.

In ST7, I would have to say my favorite new feature is the Quick View Cube.


This control sits in the lower right corner of the graphics area and will turn translucent when not in focus of the mouse, however when the mouse is in close proximity it will solidify and the individual control points will become visible.  The Quick View Cubes purpose is to give the user quick access and transitional control to common orthographic and isometric views with a single click of the mouse.  Now this doesn’t sound like a big deal, but I have watched many a user rotate a model with either a 3D Connexion device or mouse and then invoke the Common Views control which would automatically set the model square to the world using the nearest orthographic view and then close the command.  Now, they can either rotate the model with the Quick View Cube, or get it close and square it up with a single click.  Other benefits is that it has the common views printed right on it’s faces and since it always oriented in relation to the model’s orientation, it’s easy to know what common view shortcut command you want to use rather than assuming your picking the right one and finding out after it rotates to the wrong face that you should have used another.

The Quick View Cube has a few setting that can control appearance attributes like whether it is shown at all, size, which corner it is in, color, opacity level, or triad display.  These setting can be accessed by right mouse clicking on the control and selecting “Settings”.



So like I said, it’s the little simple things that I seem to be my favorite because they take something that is seemingly mature and add a new twist to it, which ends up yielding a huge user benefit.

Friday, August 15, 2014

Solid Edge Replace Part Options

If you are not familiar with the Solid Edge Replace Part command, it is an Assembly based command used to do what the name implies… replace a part or sub-assembly with another part or sub-assembly.
In past releases of Solid Edge, the Replace Part command was a solo act that had the ability of replacing a single part or sub-assembly occurrence or all occurrences of that selection with a user specified replacement part or sub-assembly that already existed.
With the release of Solid Edge ST5 and subsequent releases, the Replace Part command was actually expanded into 4 different Replace Part commands, each with their own specific capabilities.



Replace Part

Replace Part is similar to the previous Replace Part command in that it is used to replace a part with one that has already been created, however it was expanded to allow not only the selection of a single occurrence or all occurrences of the selection, but also allows a user to select different parts and/or specified number of occurrences of those selections to replace, however they will all be replaced with a single existing part or sub-assembly that you select.  Once the selection is accepted, you are presented with a Browse dialog used to locate the existing file to be used as the replacement.



Replace Part with Standard Part

Replace Part with Standard Part is a new option that allows replacement of selected parts with a part out of the Standard Parts library.  What makes this unique is that it invokes the Standard Parts selection dialog used to browse the Standard Parts Library.  NOTE: The Standard Parts Library is an optional component that is not installed by default.

Replace Part with New Part

Replace Part with New Part is a new option that allows replacement of selected parts with a part that does not yet exist.  Once the selection is accepted, you are presented with a form to select a template, specify a filename and a storage location.  Selecting the Create Part button will create a new part and add it to the assembly in the same location as the part being replaced.  You can then edit it in the context of the Assembly to create whatever geometry you wish.


Replace Part with Copy

Replace Part with Copy is a new option that allows replacement of selected part with a copy of the selection.  Once the selection is accepted, you are presented with a Save As form to save the copied selection to a new file.  Once the Save As form is dismissed, the selected component is replaced with the new copy.  NOTE:  This is the only Replace command that allows a single part to be replaced, however it will still allow single, multiple, and all occurrences of that part to be replaced with a copy of it.

Friday, May 30, 2014

Solid Edge ST7 3D Sketch… Why it isn’t exactly new.

Solid Edge ST7 introduced a new feature called 3D Sketch, but 3D sketching in Solid Edge isn’t exactly new…

Solid Edge has had a couple of add on packages for several years called XpresRoute and Harness which both have a 3D sketch tool included, but it could only be used for those modules.
image

Also, all of the 3D environments in Solid Edge have had the Keypoint Curve and Curve by Table features which are also a form of 3D sketch but work by defining points to run a curve or sketch elements between, and of course you could always create a couple of intersecting 2D sketches and generating the 3D intersection curve between them but occasionally you would run into situations where a sketch would have to double back on itself causing issues with the intersection curve generation.


So what is new about the ST7 3D sketch?

ST7 3D Sketch is a new environment that creates a “3D Sketches” node in Pathfinder and each 3D Sketch created becomes a feature underneath it.  It contains some of the prior functionality of the 3D sketch tools in the XpresRoute and Harness modules, but also adds some new capabilities such as a  cursor with 3D alignment axis', the new sketch keypoint/dimension feedback, plus a volumetric feedback indicator to let you know if you are drawing within an XY plane or also translating in the Z direction (2D box vs. a 3D box).  Also expanded are the types of elements that can be created, the number of editing tools as well as relationships, and other properties such as Styles/Colors and Intellisketch settings (although 3D capable).
image

So in conclusion, while the ability to create 3D sketches in ST7 isn’t completely new, the ST7 3D Sketch feature is, and it exposes some prior “add-on” capabilities to the the general application along with some new capabilities that simplify use and provide needed feedback to the user to create fast and accurate 3D sketch geometry easily.

Tuesday, May 13, 2014

Solid Edge Adminstrator

QUESTION: You have a group of users using Solid Edge, you ask them to all use the same settings for consistency, but there are so many that it's tedious to keep track of and not everybody agrees with all the setting choices so some don't comply... What's an administrator or team leader to do?

ANSWER:  Use the Solid Edge Administrator tool!

The Solid Edge Administrator tool allows someone to create an Options.xml file that will control various setting such as User Templates, Hole Table information, data management settings, etc...  There is actually a long list of items it controls.  You can set defaults that the user can override if desired or you can lock the settings preventing the override.

Once and Options.xml file is created and located on a network share, have every user reference it in their File Location options, and all setting controlled by the Options.xml will be automatically set.

The Solid Edge Administrator tool is not meant to control a single users settings or meant to be used by everybody.  This should only be installed and used by someone who is an administrator or otherwise has the right or need to set the standards that all others must follow.

To use the Solid Edge Administrator tool, you have to install it from your distribution media or downloaded product.  The file is called "SEAdmin.exe" and is located in the folder called "SptTools".  To install, simply copy the file and place it in the Solid Edge installation subfolder "Program" which will typically be "C:\Program Files\Solid Edge STn\Program".
Once installed, simply run it.  It will open in a table format listing the Option on the left followed by Allow Override, and the Value columns.  Make the changes you wish to control and then Save the file to a network share location that all your users have "Read" access to.  If you wish to have multiple Options files, you can give them unique names, it is not important to keep the file named as "Options.xml".

To have your users set this in their Options, have them open their Solid Edge Options and select the File Locations section. Select the line labeled "Solid Edge Admin" and click the Modify button at the top.  In the resulting Browse form, click in the "File name:" field and type the UNC path to the shared folder and option file name, and then the Open button.  Solid Edge will automatically read and change the settings at this point and now the settings are controlled by the options file.  You will notice that any options that are set to not allow override cannot be modified and any that do allow override can be.

Please note that Solid Edge does not check the Options.xml file at anytime after it is initially set.  If the administrator changes the Options.xml file later, each user must go into their File Locations area of the Solid Edge Options and highlight the Solid Edge Admin line and then click the Update button to reread it and apply the new settings.

I hope you find this post useful.