Taking Note of Inventor

Well, it looks like we've reached the last post of the year. So while reflecting back on 2008, I also started thinking about the 'Ghost of Inventor Releases Past'.

My memory fell upon a tool that I haven't used in a while, although it definitely has some benefits.

The Engineer's Notebook.

In essence, it's just a 'sticky note' inside your Inventor files, and while you can live a long, prosperous life without using the tool, it can be one of those helpful things that just might be useful in the right situation.

How to use it:

When you're in an Inventor assembly or part file, right click on the name of the file, and choose 'Create Note'.

Once you choose 'Create Note', the Engineer's Notebook will appear.



Now you can add the information you need to put in the note. In this case, I've added a note stating which model clamp we use, and that we usually have a lot of them on hand.




Now I can close the window by hitting the 'X' in the upper right hand corner of the screen. Make sure you hit the 'X' for the window, and not the one that closes Inventor.

Now you'll be returned to your Inventor modeling screen. The note will appear in the browser, and can be accessed by double clicking on the note.


By default, Inventor will have the notes show up on the screen as little yellow notes. You can turn this off by going to Tools>Application Options, and choosing the Notebook Tab. If the option are checked. The little yellow note icon will appear on screen. However, if you uncheck them, you won't see them.

I usually prefer to keep them unchecked myself. Because if you get a lot of them, your screen starts getting pretty cluttered.


That's it. Farewell to 2008, and I hope everyone has a fantastic 2009!





The KETIV Team

Suppress Your Frustrations (and drawing views!)

It's been a typical December, that is, hectic. I'm almost caught up from the trip to Vegas now (although I'd wish I'd been there to see it snow!).

Finally a chance to blog another tip again.

Have you ever had to generate a view (like the section view below) on a drawing? What if there's a case where the only view required was the section view?

The interesting part about this situation was the base view was required in order to generate the detail, so you had to have it whether you required it or not.



If you've been around Inventor for a while, you probably remember the old trick. Drag the view off the border. Of course that still left that view there, which was a little insufficient (and maybe just a little irritating!)



However, now, if you right click on a view, you can choose 'Suppress' and the view will suppress and disappear without having to be moved off the page.


Now the view goes away, and you don't have the baggage off the edge of the screen!



And by the way, if you need to unsuppress the view, right click on the view in the browser, uncheck 'Suppress', and you can return the view!



It's a little cleaner, and a little more efficient.

Happy Inventing! And Happy Holidays!

I'm back from AU!

Autodesk University is done for 2008 now. I have to say that I always learn something new, and I'm always glad I went (even though it can get pretty exhausting).

I ran into a lot of old friends and colleagues, as well as making a few more, and saw a couple of tricks too.

I'm afraid I still have to sort out some notes and get all my tricks put together. But I'm hoping to start posting some by the end of the week (really!).

One of the things I did start to get to play with is a product called Showcase. Picture being able to bring in an Inventor model, and render it in real time. Picture photo-realistic renderings that you can rotate, view, and update almost instantly (not the render in place, change rerender type).

I attached a screen capture for interest, and I'll kick up some tips at the end of the week!

There's a webcast on Showcase coming up that Kyle (our industrial design AE) is hosting. Feel free to check them out at the links below!

Showcase Your Inventor Designs – Dec. 18

Message: Accelerate your design review process with high end, easy-to-use rendering.

Showcase Your SolidWorks Designs – Dec. 18

Message: Showcase works with Solidworks.

Plus a couple of pictures from AU (sorry for the bad quality, I had to use my cell phone).


Rotating models by touching the screen directly. It's like a giant I-phone!


Sitting in one of the classes. I think this is JD Mather's importing neutral formats course!

Off to Autodesk University!

I hope everyone had a great Thanksgiving Holiday. I had a great holiday, but as usual, they always seem a little too short.

This week, it's off to Autodesk University in Las Vegas for more courses, and a chance to see other users and exchange ideas.

I'm hoping to blog from the event, and hopefully share a trick or two that I might learn.

I'll see everyone when I get back!

Going out for a Joggle (revisited)

This is actually a repost of an older post that, well, needed quite a bit of revamping. I hope everyone finds this a better explanation than the last one!

Creating a joggle in sheet metal isn’t a difficult task once you know how to approach it. The following steps will describe how to create a joggle using a combination of two different face tools.



Step 1: Using the face tool, create your first feature.









Step 2. Create a sketch on top of face completed in Step 1.


 





Step 3: Create a new rectangle (or other shape), on the plane, making sure to make one edge is colinear to the face created in




Step 4: Create a face using the sketch created in Step 3. Make sure you use the following settings:

a. The Face adds its thickness in such a way, it creates a step.

b. The Bend button is and the edge of the previous face is selected.









Hit Okay, and that will complete the joggle.

In other KETIV news! Our Industrial Designer, Kyle posted an Autodesk Showcase presentation on Youtube! Please take a look at the link HERE!

A quick tip on I-Part edting

Over the weekend I was playing with some I-Parts (table driven parts for all us old Mechanical Desktop guys), and found myself with a situation I thought was worth a tip.

I had a few columns that needed to have colors added to them, but inside the standard I-Part author, there isn't a tool that will let you copy colors like Excel. I was going to have to type them over again (or at best copy them one at a time).


Now, wouldn't that be nice.....

Well, you actually CAN edit the I-part table using Excel!

When you right click on your I-Part table for edit, you have two options:

1) Edit Table
2) Edit via Spread Sheet.




If you choose Edit via Spread Sheet, the table will open up in Excel and you'll have all the editing functions of Excel available to you. That includes things such as using formulas, and the editing functions, such as copying cells in mass (like below).



If you dive deeply into I-Part Tables, these tools can be really helpful when performing larger edits!



Happy Inventing, and on this Veteran's day, thanks for those who serve.

Finding Your (Home) View

In Inventor R2009, we saw the view cube appear and 'Home View' replace 'Isometric View' inside the right click menu.



But what happens when we need to define a new Isometric view? With our common view gone, now what?

There is still away. Choose a new view using your View Cube, right click on the View Cube, and choose 'Set Current View as Home'.

You can select from two types of home views (From the Inventor Help on the topic).

• Fixed Distance: Sets a Home view that defines both the direction of the view and the extent of the model that fills the view.
• Fit to View: Sets a Home view that defines the direction of the view and the extent is always ‘view all’. The initial Home view of Legacy documents is set to Fit to View.

Now when you right click and choose the Home View. The that view will be redifined to what you want it to be.

A big difference between R2009 and its predecessors is the home view can be any view, not just isometrics like in earlier versions.

In KETIV news:

For those who are going to be at Autodesk University in Las Vegas starting December 2nd, look up the classes being held by two of my colleagues, Nicole Morris and Mike Carlson! I'm sure there's a lot of great information they can offer!

Mike's Class

Stop Stringing it! Digitally Prototype those Wires and Harnesses

Learn to use Inventor Routed Systems to Digitally Prototype your wires and cables. Stop using the "old school" method and add more value to your mechanical design. Time and money have been wasted on electrical design and now you can virtually eliminate that waste. No more issues with tight radius bends and rework of mechanical components to allow proper clearance of for cables. Learn how to communicate with AutoCAD Electrical using XML imports and exports. Finally, document those designs effectively for manufacturing with nailboards, run lists, and cut tables.

Nicole's Class

Unleash the Spreadsheet

Learn how to increase the power of AutoCAD Electical using spreadsheets. Automate, populate, and stimulate your drawings with software you already know how to use. Learn the ins and outs of creating data outsite and brining it into AutoCAD Electrical. See how many designers use spreadsheets to plan a project and reuse data effectively. Understand the fundamentals of these tools allowing you to cut production time in half.

Become comfortable with how spreadhseest are handled in AutoCAD Electical so that youc an create your own versions. Samples and Datasets included.

One last note. Happy Halloween!

Playing Your (Drawing) Scales

Just a short tip on one of those 'little' things that comes up from time to time.

I came across an issue where someone was placing an AutoCAD drawing in Inventor (via the cut and paste method), and the view pasted into the file was the wrong size.

Closer inspection showed that the view was scaled to a factor of 24.5. In other words, the part was created in mm, and had been pasted into an inch drawing (or vice versa).

In any case, here's a quick way to fix those when they come up.

Once you've copied your geometry from AutoCAD, Paste it into Inventor as you normally would.


You'll see the preview box, however, before you left click to place the view, right click again.


Right click and choose 'Paste Options'


Once you choose Paste Options, you'll see the options screen that will let you specify what units the sketch should be in. Pick the units, and this should fix the issue!



Thanks again for coming to Autodesk Manufacturing Academy (AMA). Feel free to swing by our website here, and take a look at some pictures.

I Prefer Perfect Perforations (in Sheet Metal)

First of all, thanks to everyone who came to the Autodesk Manufacturing Academy. It was great to see some old friends, as well as meet some new ones!


Here's an interesting little problem a user ask us during the sheet metal class (I'm sorry but I dont' remember the name!).

How can perforations be created on a sheet metal part in such a way that the geometry can be cut on a CNC machine of some type (laser, water jet, etc).

One of the simplest solutions would be to create a transparent texture that would visually show the perforations, but that doesn't give you any geometry that could be cut by the machine.

Another method would be to try to model the perforations and use a pattern to wrap them aroudn the folded model, but that could be tricky, and if the pattern gets to be large, could cause a performance issue.

Another option a bit of a marriage between the two options. You can create a folded model without perforations, but add them to the flat pattern using the modeling tools there.

The perforations won't show in the model, but you'll have them in the flat where the CNC machine will cut them.

Here's the folded model.


Here's the flat pattern, with some sample perforations added in the flat.





In this method, you achieve a balance between the need for and accurate part representation for the machine, while eliminating the extra effort of trying to maintain the pattern on the folded model!

And if you still want it, you can still use a texture for something representative on the folded model!

Meet at the (Theoretical) Intersection

Every once in a while you may need to create a dimension on a drawing where a part's sharp corner would be, if there weren't a fillet, round, or chamfer in the way.

Here's a quick description of the steps used to get there from here.

First, we have the part with chamfers breaking up the theoretical sharp corners on our drawing.



Step 1: Start your General Dimension tool as you normally would, and choose the first line you want to dimension (the first half of the intersection).


Step 2: Right click, and choose 'Intersection' from the menu that appears.


Step 3: Hover over the second line in your intersection. You'll see a preview appear showing you where the dimension will anchor. Onse you see this preview, you can left click to place the first extension line of your dimension.


Step 4: Click the second edge you want to dimension (in this example, another 'theoretical intersection') . The dimension may place 'unusually', since it will initially think this is where we want our second extension line placed.

We're going to fix this by telling the second extension line to anchor from the theoretical intersection.



Step 5: Right click again, and choose 'Intersection' from the menu.




Step 6: Just like earlier, choose the second edge that will comprise your intersection. A second preview will appear.


Step 7: Select the edge, and your dimension will be placed.


Happy Friday!

For those who are going to be at AMA on September 25th, I'll see you there!