Search This Blog

Loading...

Friday, April 4, 2014

Inventor Tube & Pipe Wish List Part 2

lHello again all you happy people.












Sorry, I just like Droopy.

Anyway,  welcome to Part 2 of my Autodesk ® Inventor Tube & Pipe wish list.  I revamped the first post in this series to include links to the Autodesk ® Discussion Forum Idea Station posts for these suggestions, so I will do the same here.  Ready to go?

Tube & Pipe Branching

This request has actually been moved to the "Under Review" state in the Idea Station, which means that Autodesk is looking at whether this CAN be done, and SHOULD be done.  Progress!  Basically this is what I am asking for.  Currently, in Tube & Pipe, you create a branch by adding a branch fitting into an existing route, and then beginning a new route from the outlet of that fitting.  This works just fine, until you need that branch to line up perfectly with another pipe run, or a piece of equipment whose location is fixed.  See the image below; I need a line coming from the outlet of the pump and intersecting the main trunk line shown.  If I place a tee in this line, I would need to have an external reference point in my route to constrain the tee's location to in order to ensure it lines up with the pump suction.  If the pump moves later, there is no guarantee that this reference point would move with it, and would result in a failed route.

Branch Location

My proposed solution is one I have seen in another piping program.  It would be nice if we could run a line from the suction nozzle of the pump and have it intersect the main line shown, and have Tube & Pipe place the tee automatically.  Perhaps this would mean that in our Tube & Pipe styles we would need to specify a branch fitting as well as the elbows we need to specify now.  I would be OK with that!  This could even work in the context of a single route, creating branches on the fly as needed.  If done in conjunction with one of my other proposals; the ability to have a route reduce in size; the branch fitting could even be a reducing tee, for example.  Here is a link to the Idea Station post if you want to add your Kudos.

Tube & Pipe Branching

Content Center Parameters Propagated to Tube & Pipe


A little over a year ago I posted an idea to the Idea Station about a problem I was experiencing with getting column information out of the Content Center Family Table and onto my part models in Tube & Pipe.  Here is a screen shot of the post:

Idea Station Post


I was going to include this in this wish list, but in the last few days I have had some great success on a work around for this problem.  Instead I think I'll end this whole thing on a positive note and share what I've figured out in case it will help you.

To sum up what I was after, I wanted to get the same information onto the pipe spool model regardless of whether it was placed as part of a pipe run, or simply placed as a stand alone part.  The out of the box behavior was different in Tube & Pipe than when placing it loose in an assembly.  I wanted a concatenation of the spool type, nominal size and length.  The work around starts at the part level. I placed a pipe spool from the Content Center, "as custom", and saved it as a stand alone part.  I opened up that part file and looked at the model parameters.

Pipe Spool Part parameters
In the parameters I scrolled down to "length".  This parameter was first created as a part of the original iPart which was authored and published to be our flanged pipe conduit.  For help on creating and authoring your own custom pipes, see this Help document:

Author a pipe iPart

I set the length parameter to be exportable, then right clicked on the length value and selected "Custom Property Format".

Custom Property Format
For my needs I wanted the value to show up in my iProperties and in my Bill of Materials as fractional inches.  I unchecked the Units String so that the "in" would not show up as a part of my file names later.

Custom Property Format Dialog Box
With these changes tucked away, I saved and closed the part, making note of where I saved it for the next step.  In Inventor still, I went to the Manage tab and opened the Content Center Editor.  Finding the family for this pipe spool in Tube & Pipe\Conduit\Pipes, I right clicked and selected "Replace Family Template".  When the file dialog box opened I navigated to the location of the spool I had just modified and selected it.  After a few moments (with my fingers crossed) I got the satisfying "Published Successfully" message.  These changes to the parameters had now been propagated to the Content Center Family.

Next, I edited the Family Table for this pipe part.  Now, normally I use one column in a part family table to populate both the file name and the BOM description.  I do this by mapping the file name column to "Project.Description" under Column Properties.  For these pipe parts, however, this didn't work.  The fact that I was getting different results in Tube & Pipe, versus placing the pipe as a stand alone part made it necessary to use two different columns to populate file name and description.  File name is a standard CC Family table column, so for this one I chose an Expression as shown in this shot:

File Name Column Properties.
To edit this, you right click on the column header and choose Column Properties.  The Expression string is hard to see but here is the text:  {DESIGNATION}&" ETFE SPOOL x" &{length}
Designation is set to our sizes for this pipe, expressed as 3 or 4 digit size codes (1" - "100").  The Length column has been set up as an Expression column as well as shown here:

Length Column Properties.
This allows Tube & pipe to place these pipe spools at any length in this range.  Note it is mapped to the iProperty Custom.Length, which will push the value of Length out to the part as a custom iProperty.

For the Description, I chose a column we were not really using for anything else, but you could just as easily create a new column for this.  In my case I used Stock Number.  I set up the Column Properties as shown here:

Stock Number Column Properties

Note how this is mapped to Project.Description to populate the part iProperty.  Again the text of the expression is:  =&{DESIGNATION}&" ETFE SPOOL x <length>"  This is slightly different than the File Name.  The "carrots" around length here will cause the resulting string to populate the part iProperties as an expression there, using the value of the custom iProperty "Length" as a part of the Description.  This will ensure that if the pipe route changes later on and the length is different, the part iProperty for the description will update automatically to the new length.  This was something I was trying to do for quite some time and finally hit on it.

So with this somewhat lengthy process, I was able to force my pipe spools to come into Inventor with the correct file name and iProperty information, regardless of how they were created.  A shot of the iProperty dialog for my test pipe looks something like this:

Pipe Spool iProperties

Note the file name along the top has the size, the type of pipe spool and the length.  In the Description field, I have set it to show you what the expression looks like, the value for it is the same as the file name.  Now, it is important to note that when routing pipes using Inventor Tube & Pipe, your pipe spool file names will be auto generated.  You can set your Tube & Pipe setting such that you will be prompted for conduit file names.  To do this, right click on the "Tube & Pipe Runs" main assembly in your Inventor browser window, and select "Tube & Pipe Settings", then check the appropriate box.  I do this so that I can add the job number to each spool as a prefix.  It's a lot of work up front, but I'm always glad I did it later when I need to use Copy Design.  Also note, that you can modify the file name that is generated by placing a pipe spool outside of Tube & Pipe, if you place it "As Custom".

Well, this went from a wish list to a tutorial, and I'm sorry if I got long winded... but I hope there is something in here you all can use.  As for me I think it might be time to call it a week.

Enjoy!

“Autodesk® screen shots reprinted with the permission of Autodesk, Inc.  Autodesk ® , AutoCAD ® , DWG, the DWG logo, Vault ®, Autocad Electrical ® and Inventor ® are registered trademarks or trademarks of Autodesk, Inc., and/or its subsidiaries and/or affiliates in the USA and other countries.”  Programs and programmers' information used with permission.  Thanks guys!

Wednesday, March 26, 2014

Inventor Tube & Pipe Wish List Part 1


Hello out there!  Anyone still with me?  It's been a long time since I've had the time to post.  Anyone who has seen my posts on Twitter or Linked In or on the Autodesk ® Discussion Forums knows that I am heavy into using Inventor's Tube & Pipe module.  You may have also seen that I make no secret of my belief that this module is long overdue for a major facelift.  It's a good system, but it is also responsible for more than a few of the grey hairs on my head!

I thought I'd put forth a few of my ideas for how this could be improved, based on my real world pipe design experience.  This entire post will be my own opinions and thoughts, backed up with some snazzy pictures, and links to the Autodesk ® Forums Idea Station posts, where applicable.  So... let's dive right in!

Changing or resizing fittings on existing Pipe Runs.

Inventor Tube & Pipe works very well with few issues when you are designing a pipe run that is made up of a length of pipe with fittings placed inline along it, allowing spaces between the fittings.  An example of an easy pipe run:

Example of smooth pipe route.
In this example, the elbows have all been determined by the route and were placed when the route was populated.  They will not move or change their orientation unless I edit the route and change the direction that way.  The fittings that have been placed inline may be rotated in any way I choose, since the axis of rotation is the center line of the route.

Sometimes, however, the pipe runs I need to deal with do not have these nice long spaces between fittings populated by a pipe spool piece. In many of our designs I am dealing with a pipe run where the fittings are placed face to face with other fittings, with no intervening pipe length.  The axis of rotation for any given fitting, now becomes the connection point on either end of the fitting.  The more connection points, the more potential rotational axes.  Example:

Face to Face Pipe Run
In this example, the pipe segments you see are actually flanged pipe segments that we created, since a lot of our piping is plastic lined steel piping, and each spool piece is hand made to a specific length.  Rather than place each one as a fitting, we wanted the flexibility to change the lengths on the fly as the design is progressing.  I created a base spool as a pipe conduit in Inventor and placed it into several Tube & Pipe Styles.  This will be covered in greater detail in another post I am formulating right now... look for that in a week or so. Anyway, notice that the majority of the fittings have no intervening pipe segments.  Here is where the "fun" begins.

Pipe fittings that have been placed using fitting to fitting connections, rather than being placed inline on a route, have an annoying habit of wanting to change their orientation when they are modified in any way.  If you attempt to change the size or replace the fitting with another similar fitting, (let's use the elbow on the left in the image above for this discussion) the new fitting tries to come in at a different rotation than the fitting being replaced.  If this fitting is connected on both ends, this will cause a general "replace fitting error" message to pop up.  If you are new to the program you might have no idea what the error means, or what the problem is.  Breaking the connection on one end only allows the change to be executed, but the results may be... interesting at the least.  The best solution, (and I say this sarcastically since this is no solution in my mind, but rather a workaround) is to break the fitting connections on both ends of the fitting.  Then attempt the fitting change again.  With this workaround the fitting should replace or resize fine and stay in place.  (but wait, there's more).

Now that the fitting replace or resize has been done, it has to be reconnected to the rest of the assembly using the "Connect Fittings" command.  Looking back to the image above, (remember it was the elbow on the left we used in this example), let's assume that we reconnect the elbow to the tee fitting in the middle.  The fittings will connect with no problem, but to our surprise the elbow has rotated up 90°.


Fitting Rotated After Reconnecting

Now we have to supplement the Connect Fittings command with Edit Fitting Orientation to rotate it 90° back down to it's beginning orientation.  Now we have to connect it back to the pipeline.  Using the Connect Fittings command again to select the elbow and the pipe segment.... Tube & Pipe creates a Pipe Route loop to connect between the fitting and the previous pipe segment!

Pipe Route Looped Onto Itself.

So, after a few more taps of the Undo button, we have to actually delete the pipe segment and route a new segment starting from the elbow out to whatever length we need.  Once that's in place we can use Connect Fittings to connect the new segment to the next fitting in the line, and finally... after all of these steps, we have successfully changed the size of one fitting in our pipe run.  Now we can proceed to change any other fittings that need to be replaced or resized.

This to me is a huge waste of time for any designer, and therefore money.  My proposed solution is hard to define since it depends on what the root cause of these issues is.  But it seems that there are obstacles to the freedom and flexibility that a designer needs to be able to make changes to a design as a project unfolds.  The fix may be in question, but the desired result is not.  Fitting to fitting design is a large part of a piping designer's real world experience.  The ability to quickly change, resize or otherwise modify these fittings in place, without causing rework to the rest of the pipe run or any other pipe runs attached to it, is a must have in my opinion.  Design criteria change fast, the designer needs the ability to change a model as fast in order to keep up.

Looking back, I find that I have posted more than one Idea about this problem in the Idea Station.  If you feel this pain, or even if you feel some sympathy, feel free to visit these posts and offer your Kudos.

Pipe Connections Easier To Change....

Tub e & Pipe Pet Peeve #652


Changing Pipe Sizes in a Pipe Run.


For a brief and ill advised period a few years back, my company switched to Pro Engineer for their Pro Piping module.  There is little I can say good about Pro Piping, in my humble opinion.  But there is one (and only one) thing it did better than Inventor's Tube & Pipe.  Pro Piping had the ability to change pipe sizes WITHIN a single route, automatically.  Let me break it down a little.

Fittings in Pro Piping were authored very similarly to those in Inventor.  They didn't call it authoring, but I cannot recall what they did call it.  (The bad memories are fading)  The main difference was that instead of defining an insertion work point and axis for each connection, the user defined a coordinate system, making sure that the "Z" axis was facing in the direction of the connection.  These User Coordinate Systems were then given a Size parameter.  When routing pipe, the user selected a spec which was similar to Inventor's Tube & Pipe Styles, with one major difference.  The spec did not have any size associated with it, it called out the material and allowed fittings.  The size was determined by the size parameter on the fittings themselves.  As long as the fittings and pipe which were allowed by the spec existed in the size currently being routed, the route would populate.  Example:  If you began a route at a previously placed Pipe Flange, which had a 2" parameter on the open port, the route would assume 2" as the nominal size.  Any fittings placed in the line would assume 2" as well.  If a reducer type fitting was placed inline, which had a 1" port on the other end, the pipe route and any existing fittings downstream of the reducer (as long as they existed) would automatically switch to 1" as determined by the size parameter on the reducer.  if the program ran into a situation where a fitting or pipe to be reduced did not exist in the fittings allowed by the spec, the program would prompt the user as such and ask for a substitute to override the spec.

In Inventor, the same situation has two possible solutions.  One is to route the 2" pipe up to the assumed location of the reducer and stop.  The reducer fitting would be placed manually and connected to the end of the 2" route, and a new route created for the 1" pipe downstream.  The other method is to route the entire pipeline as 2", place the reducer, and then manually change size on all pipe and fittings downstream.  The problem with method 2, is that nay changes made later will revert the pipe segments downstream of the reducer back to the 2" specified in the Tube & Pipe Style, necessitating that the user change them manually again.  As in the previous section, this does not allow for the flexibility needed by designers in the real world as things can change rather quickly.

Here is a link to the Idea Station post for this suggestion:

Reduce Within A Pipe Route

I'm going to end this now and call this part 1, so that it does not get too long and bore you all to tears.  I have more ideas and I'll work on compiling those into a part 2 soon.  In the meantime....

Enjoy!

“Autodesk® screen shots reprinted with the permission of Autodesk, Inc.  Autodesk ® , AutoCAD ® , DWG, the DWG logo, Vault ®, Autocad Electrical ® and Inventor ® are registered trademarks or trademarks of Autodesk, Inc., and/or its subsidiaries and/or affiliates in the USA and other countries.”  Programs and programmers' information used with permission.  Thanks guys!

Wednesday, February 19, 2014

AutoCAD ® Electrical Symbols on Tool Palettes

Hey there!

Wow... this one has been a while coming.  I posted a teaser a few weeks ago thinking I had the question answered, and all I had to do was write the post.  Then a few more hours of testing turned up some show stopping problems and I pulled the teaser... dejected and frustrated.

Some of you may not know what I'm talking about, so here is some background.  AutoCAD ® Electrical has a massive symbol library of schematic symbols for electrical, hydraulic/pneumatic and for P&ID's.  It also contains a huge library out of the box of electrical panel footprint symbols, for creating physical panel layouts.  All of these libraries are fully customizable.  you can add to them, subtract from them and even modify the existing symbols through the Symbol Builder tool in the program.  These symbols are all accessible through an Icon Menu that has multiple screens and nested menus.  This is also manageable through the Icon Menu Wizard tool.

Autocad Electrical Icon Menu

Lots of flexibility there, but not the most user friendly interface, in my humble opinion.  Of course, it may just be that this is not the way I am used to doing things, coming from so many years of using plain AutoCAD ® for all of our schematics.  It may even go all the way back to having all of my symbols right in front of me on one of those massive tablets we used to use back in the day.

AutoCAD Menu Tablet R14

Anyone remember these?  They could be configured to include custom commands or symbols pretty much anywhere on the tablet, but primarily in the empty top section.  You could edit the menu file, and there was a drawing of this tablet screen where you could add or delete or move things around.  Plot it off, tape it down and off you went.



These days my preferred method for inserting blocks is the tool palette.  if you have not looked into all that tool palettes can do for you, I highly recommend you do.  Take a look on the Autodesk ® University website, there are several online classes from past AU's that are available for download.  In Autocad we have several palettes that contain our symbol libraries for both electrical and flow diagram schematics.

A little over a year a go, we made the decision to switch our electrical schematics to AutoCAD ® Electrical.  This was mainly due to the fact that it was added to our Product Design Suite.  We had it.... let's use it.  So, I set about learning the basics.  I am by no means an electrical designer.  It's a language I simply do no speak.  We've gotten pretty proficient at using the AcadE to create our ladder diagrams and panel layout drawings, but I know I have a long way to go toward leveraging the real power behind the software.  Meanwhile, I learned that AcadE can also be used to create P&ID's.... a large part of our business.  By using the same software for both schematics, they can be linked in a single project and tag numbers on the P&ID can be associated to tags on the electrical diagrams.

Well, project work gets first priority here, as you can imagine.  Have to pay the bills after all.  Special projects get more of a back seat.  So, it's been quite a while since I first looked into this conversion.  Now that I am jumping into it with a little bit of time to work with, I decided to try to figure out a way to put the P&ID (and eventually electrical) symbols onto our tool palettes to simplify things.  After several failed attempts using a variety of methods, I was ready to throw in the towel and embrace the icon menu path.

So, once I started down that road, I posted a question of the Autodesk ® Discussion Forums for AutoCAD ® Electrical, asking if it were possible to dock the icon menu somewhere so I wouldn't have to keep opening it up every time I wanted to place a symbol.  A very talented individual, who has helped me in the past but whose real name I do not know, suggested that I take a look a the API help for AutoCAD ® Electrical.  Now, I've heard about the API... but I never thought I would ever touch that area.  But, on his advice, I looked under the Help menu and saw "Additional Resources".... under which I saw API Help, and found my way into a place that can only be described as a treasure trove of customization tools.  I don't know why I never thought to look here before.

It wasn't long before I found a tool that might do what I was looking for, and it was so simple that I laughed at all of my pathetic efforts to date.  I had no idea what I was looking for.  I figured it might be in the section under Schematic Components, so I opened that section of the help up and found a list of commands and a description of what each one did, and examples on how to use them.  Working my way down the list I found this:

AutoCAD ® Electrical AutoLISP Reference
The description shows that this is a way to call the Insert Component command from the command line, and skip the Icon Menu.  You provide the block name, and specify a value for the parameters following it.  So simple.  I tried it out and it worked from the command line immediately.  If it can work there, it can work on a tool palette.  I added a command to my test palette, and put this as the command string:

(c:wd_insym2 "HDV1_VLV_BLK" nil nil 1)

The block name is in parentheses, and if no path is given, the system will use your preset search paths.  The two "nil" parameters allow for user input for the insertion point, and next set the scale to 1 for the block.  The option 1 at the end tells it to open the component editor as soon as the block is placed.  This does exactly what the icon menu does.... right from the convenience of my tool palettes.  I was a very happy man when I saw this.  Now I just have the tedious task of turning all of my old symbols into smart AutoCAD ® Electrical symbols, and creating the commands on my palettes.... I should be done by..... summer?  Maybe?  Meanwhile, I'll have to dig back into that API and see what other trouble I can get myself into.  More later?

Enjoy!

“Autodesk ® screen shots reprinted with the permission of Autodesk, Inc.  Autodesk ® , AutoCAD ® , DWG, the DWG logo, Vault ®, Autocad Electrical ® and Inventor ® are registered trademarks or trademarks of Autodesk, Inc., and/or its subsidiaries and/or affiliates in the USA and other countries.”  Programs and programmers' information used with permission.  Thanks guys!

Friday, January 17, 2014

Populating Autodesk ® Inventor iProperties from the Content Center

Did you know you could do that?  It's pretty powerful, and actually powerful easy to do once you know the trick.  You can make any column in an Autodesk ® Inventor Content Center family table send metadata out to the iproperties of the generated parts.  What you do with that metadata after that is up to you.  In my setting, I use a lot of it to map to properties in the Autodesk ® Vault Item Master.

This can be done with either custom content that you have published from your own iparts, or with standard content that you have copied to a read/write library in the Content Center.  When you create an ipart in Autodesk ® Inventor, any iproperties that you add to your ipart table as columns will automatically map themselves back to that iproperty when you publish the ipart to the Content Center.  For standard content that you copy to your read/write library, however, you may find that only certain properties (Part Number, for example) are already mapped for you.  Anything else you want to map, or any mappings you want to change around, you will have to add yourself.

As an example, I've chosen one of my pipe fittings, a CPVC 90 degree elbow.  This was published from a custom ipart that we already had modeled up years ago.  However, now, there is information I would like to have sent to the part's iproperties in order to trigger some Autodesk ® Vault properties when the part is checked in and added to the Item Master.  I want to take the "Member" column metadata (which came right form the ipart table), and map it to the iproperty "Subject".

To do this is very easy.  On the Manage tab in Inventor, pick the "Editor" button to open the Content Center editor window.  Navigate to the CC family you wish to edit, and right click on it, selecting "Family Table" to open the family table editor.  Locate the column whose metadata you want to capture.  Right click on the column header, and select Column Properties.  You should see a section titled "Map To Inventor Property", with a pull down below it.  Select the pull down menu to see a list of available properties to map to.  Note that an iproperty in Inventor may only be mapped from one Content Center column.  If the property you wish to map to is not visible in this pull down list, it is probably already mapped from another column somewhere in that family table.

Map To Inventor Property

Once you have mapped all of the columns to properties that you need for that family, select OK at the bottom of the editor. You should see a pop up which tells you "Published Successfully to the Selected Library".  Hit OK again and close down the Content Center Editor with the "Done" button on the lower right.

Now to test your results.  I suggest creating or opening a dummy assembly file for the testing, you'll see why in a moment.  When you first use a Content Center part in Inventor, a part file is generated and placed in your default Content Center location, as determined by your Application Options file settings.  Every subsequent time that you place that same part, it retrieves it from that folder in it's current form.  So, to test your modified family, you need to know if the parts have already been generated or not.  In your dummy assembly, use "Place from Content Center" on the Assemble Tab.  Place an instance of the family, and look at the part's iproperties.  If this is the first time the part has been generated, you should see the mapped property filled in.

 
iProperty Successfully Populated



If the part has already been generated, the iproperty will remain blank, or will retain whatever value was in it before.

iProperty on Previously Generated Part

So now the question is, how do I get this part to accept the new information from the family table?  Easier than you think.  The way you do this will depend on the size of the table, and the number of instances you need to update.  In a relatively small family I will do the update right here in my dummy assembly file.... get it over with.  For a very large family I tend to use this update tool on my production assemblies regularly, to catch any out of date content parts as they come up.  Anyway, here is what you do.

Place as many instances as you plan to update, and then save your assembly file.  It must be saved before you can update the parts.   On the Manage tab, select the "Refresh" button, normally located next to the Editor button you used earlier.

Refresh Standard Content

Click the Refresh button at the bottom of the dialog box, and Inventor will update the Content Center part with any new information or changes made to the family table.  If you use Vault, you will be prompted to check out the parts in question so that the changes can be saved to the Vault file as well.  Once the process has run, check the iproperties on the part once again.

Updated Content Center Part

You can also add columns to a Content Center family if there is information you want to map to an iproperty which is not already in the family table.  Adding columns and creating expressions in family tables.... that's for another day.  ;)  So I hope this was helpful in getting data from a Content Center table into an Inventor part's iproperties.  And as always....

Enjoy!

“Autodesk® screen shots reprinted with the permission of Autodesk, Inc.  Autodesk ® , AutoCAD ® , DWG, the DWG logo, Vault ®, Autocad Electrical ® and Inventor ® are registered trademarks or trademarks of Autodesk, Inc., and/or its subsidiaries and/or affiliates in the USA and other countries.”  Programs and programmers' information used with permission.  Thanks guys!

Monday, January 13, 2014

Share your ideas!

Good morning!

I've been away for a while again.  Working hard on CAD drawings and Vault cleanup.  As some of you know I spend a lot of time in the Autodesk ® Discussion Forums, either asking for advice or offering it when and wherever I can.  I quite often see people posting, as questions, thoughts on what they perceive as features that are missing from their CAD software.  It occurred to me this morning while answering one such question, that many people are not aware of the Autodesk ® Idea Stations.

While not every forum currently has one of these, there is one for both Autodesk ® Inventor and Autodesk ® Vault.... which are the two areas I tend to spend the most time in.

http://forums.autodesk.com/t5/Vault-IdeaStation/idb-p/2

http://forums.autodesk.com/t5/Inventor-IdeaStation/idb-p/v1232

So, what is the idea station?  This is the place to go to post ideas that you have about functions or features you believe should be added to your Autodesk ® software in order to improve useability or to address some specific problem you are having.  This is NOT the place to go to complain about what you don't like or what the product can't do.  This would simply be unproductive, and certainly wouldn't advance your cause.  The way they work, is that you post your idea or suggestion in as much detail as possible, including pictures or screen shots or anything else that would help to illustrate what you are looking for.   For example, if your idea is posted to address a specific problem, you may post a screen shot of the problem as an example.

Idea stations are routinely looked at by Autodesk's ® development people, and they do take these suggestions seriously.  Ideas are ranked based on reader's votes, or "kudos".  Ideas that get more kudos, get more attention.  So the thing to do is post your idea and then sell it!  Post in the regular product forums and let people know you have just posted a new idea, and invite them to check it out and vote for it if they like it.  Jump on Facebook or Twitter or wherever you interface with your CAD colleagues, and post a link to the idea.  The more you sell it the better the chance it will be looked at.

Here is the catch.  There are thousands of ideas out there, and only so many hours in a day.  Some ideas may be accepted by the developers, but (believe me!) might not make it into a new product release or update for quite some time.  We have to try to remember that these people are as buried with piles of work as all the rest of us, and they are only human.  Easy to forget that since we are the customer, and expect satisfaction.  In my experience, Autodeskers ® are very receptive to productive ideas that get a lot of votes.... but it just takes time to implement these.

So go ahead and share those ideas, and if you haven't spent much time in the Autodesk ® Community forums... join up!  Lots of great folks in there willing to help you out and even a "Break Room" forum for non CAD related discussions.  It's a great online community experience.  You might even "see" me in there.

Enjoy!

“Autodesk® screen shots reprinted with the permission of Autodesk, Inc.  Autodesk ® , AutoCAD ® , DWG, the DWG logo, Vault ®, Autocad Electrical ® and Inventor ® are registered trademarks or trademarks of Autodesk, Inc., and/or its subsidiaries and/or affiliates in the USA and other countries.”  Programs and programmers' information used with permission.  Thanks guys! 



Monday, December 30, 2013

Happy New Year and Thank You!

Just a quick post to say thank you to everyone who actually visited this site this past year.  This was an experiment just to see if I had it in me or not.  The fact that so many of you read it and liked it was a bonus to me.  If I was able to help even one of you in some small way then I exceeded my expectations.

In the following year I will try to keep this going and post new ideas as they pop into my head.  I'm going to be doing some experimenting with programming so maybe I'll have some posts about my progress in that.  If you have any ideas for topics you would like to see me write about, comment on this post.  I won't make any guarantees, but if time allows (and I know something about what you are asking for...) then maybe I'll post on your topics.

Once again thanks to all of you who have read my ramblings, and I wish you all a very Happy New Year!

Enjoy!

Monday, December 2, 2013

AU2013 Live (sort of) Blog


MBS Airport Main Terminal
MONDAY:

MBS International airport.  First stop on my journey to Las Vegas for Autodesk's ® annual gala of learning, networking and technology.  As this week progresses I will be posting my thoughts and experiences for whomever may care to follow along.  Wi-Fi is weak in this terminal so.... this is about it for now.  Short layover in Detroit won't allow me any time to write so I'll see you all in Vegas!

All right! Made it to Vegas, checked in and got my cool tote bag and a sharp looking Charlie Harperesque bowling shirt with the Expert Elite logo on it!  Now I'm preparing for one of the most important events of the week.  Freshman Orientation with Lynn Allen, Autodesk ® technical evangelist and all around nice person.  I've foolishly volunteered to be a mentor this year, so first years beware!  More to come as the night rolls on, and plenty more tomorrow.  Stay tuned.

Freshman Orientation

This was part of the scene as over 1,000 Autodesk University freshman filed in for some words of wisdom.  155 mentors and several speakers shared tips and advice, and then Lynn Allen gave away a free pass to next years conference.  I didn't win.  The t-shirt gun went off several times as well to a few lucky winners.

I'm back in my room at the Venetian now and recharging all of my devices.  Getting ready for the Blogger Social Media Meetup (BSM360) later this evening.  Maybe I'll have some pictures from that later.

BSM360

BSM360

BSM360

TUESDAY:

Just a few of the shots I took at the Blogger Social Media Meetup last night.  Good times, lots of great people, free beer... but the pizza never showed up.  Hmmmm.  So after this I was pretty much ready for some sleep... still on Michigan time.  

Then this morning:

The Dining Hall

Breakfast with 10,000 new friends!  This picture does no justice to the size and scope of the meal hall.  Super friendly staff help guide you to a buffet, and then you find a table to sit at.  I try to find new people at every meal, you never know where you'll make a new friend, and that's part of why we're all here.

I'm currently finishing a coffee in one of the lounges, getting ready to find my first class.  I'll check back in soon!

Waiting For Opening Keynote

This was the THRONG trying to file in for the keynote this morning!  A sea of humanity.  The theme of the keynote was "The Answer is Outside".  Autodesk CTO Jeff Kowalski and CEO Carl Bass talked about changing our mindset and thinking outside of our normal ways if working.

Opening Keynote

Penn & Teller

Hard to see in these tiny iPod pics, but this is special guests Penn & Teller who opened the presentation with their usual wit and, of course a cool magic trick.  Sevearl companies were highlighted who exemplified thinking outside in their innovations.  For me, however, the star of the show was Iris.  Iris is a robotic camera dolly designed by Bot & Dolly using Autodesk ® tools.  Bot & Dolly created the robotic camera arms used in the recent hit movie "Gravity".

IRIS

Pretty awesome morning so far!  Lunch in the hall was tasty, and accompanied by more networking opportunities.  The only battle I am fighting so far is the Wi-Fi!  If I want to live blog in the future I think I need  smart phone or tablet!  I am literally recharging and preparing for more classes this afternoon, so.... more later!

WEDNESDAY:

It's Wednesday morning now and my dogs are barking.  A lot of walking, it makes me glad for all those hours on the treadmill.  Coffee time and a quick check in here before another long day of classes.  Last night was spent in the Exhibit Hall, visiting some of the vendor booths and hanging out in the Community Pavilion.  I wandered between AUGI and the Expert Elite kiosks and basically mingled.  Food, drinks and reggae music were the backdrop to several hundred exhibitors showing off the latest tech, giving away prizes or tossing toys to the crowd as they passed by.  There is something for everyone.  At our Community Pavilion we even have 6 classic arcade video games setup... no quarters needed!  So... upstairs now to find my first class and see what awaits me today!

My Big Prize!
THURSDAY:

I won big in Vegas!  OK, so it's only a backpack, but I never win anything!  Thursday morning... the coffee is barely holding me up.  Long day of very good classes yesterday, time at the answer bar, and then the AUGI beer bust in the Exhibit Hall.  Spent most of the evening at the Community Pavilion with my fellow Expert Elites.  Almost forgot to mention my photo op at lunch with Carl Bass, Autodesk CEO.  We had a special lunch for to celebrate the first anniversary of the Expert Elite program, it was a good time with some new and old friends.  Not to mention the best meal I've had so far this week.  As soon as those pictures are available, I'll add it here. (added 12/11)

Carl Bass and I

Expert Elite Lunch Group Photo


Breakfast this morning was decent, now getting ready for my first class.  I filled out my conference survey and got a "cool" AU t-shirt.  Big times on Vegas!  I haven't taken many more pictures because yesterday and today will basically be focused on learning.  I haven't taken my iPod to the Exhibit Hall because there is no Wi-Fi down there.  Definitely need a smart phone before next year.

I have a full day of classes today, all Autodesk ® Vault... all day.  Hoping to pick up a few tips and tricks.  As well as a sneak peak at the new release. 

FRIDAY:

Well, it's over.  I'm sitting in my room writing because it's way to early to head down and wait for my airport shuttle.  Yesterday was a very productive day of classes.  I learned a lot of great tips I need to incorporate when I get back to the office.

When classes were done, I attended the closing keynote address, which was followed by another performance by Penn & Teller.  They are very entertaining, there's no other way to put it.  How lucky were we to get a "free" performance. I tried to get some pictures, but with this IPod, they just didn't turn out.  I was too far back, and at an odd angle to the screen.  Also featured in the address was a private group building their own rocket and robotic lunar explorer, with the intent to be the first private entity to reach the moon.  They hope to launch sometime in 2015.  This could change the future of space exploration by putting it in the hands of private enterprise.  Fairly cool in my opinion.

Following the performance by Penn & Teller was the AU Customer Appreciation Party.  I stayed just long enough to eat some food and mingle with a few people I had met, and then turned in early.  Long travel day ahead and I wanted to pack and get a good night's sleep. This may be the last paragraph I can write until I get to the airport so I'll be back then.

MONDAY:

Back in the office... I've tweaked this blog a bit to clean up the mistakes my iPod made (blame it on the tech... not me).  Flights home were uneventful, thankfully.  I hope the handful of you who read this enjoyed it... I've never live blogged before so I know I can polish it up next time.  Thanks for reading!

Enjoy!

“Autodesk® screen shots reprinted with the permission of Autodesk, Inc.  Autodesk ® , AutoCAD ® , DWG, the DWG logo, Vault ®, Autocad Electrical ® and Inventor ® are registered trademarks or trademarks of Autodesk, Inc., and/or its subsidiaries and/or affiliates in the USA and other countries.”  Programs and programmers' information used with permission.  Thanks guys!