Autodesk Manufacturing & Digital Prototyping Solutions

Autodesk Inventor: Quick Tip - Degrees to Radians

We had a question come up on the Autodesk Inventor Facebook page recently and it's one that I have been asked a couple of times before so thought I'd do a quick tip - How can I change units from degrees to radians? So here you go...

If you're using the measure tool to measure between geometry all you need to do is click on the black arrow in the measure tool, select Dual Unit and then select the unit you wish to show. In the example below I already have Radians set as my default unit for angular measurements, so the alternative is Degrees:

However, if you want to change your default units so that you always use Radians rather than Degrees, you can do this quickly and easily with the Document Options.

First, just click on the Tools ribbon and select Document Options...

Then click on the Units tab and select the default units for your angular measurements:

Having this set to Radians will mean all angular dimensions within sketches and measurements (using the Measure tool) will be shown by default in Radians.

If you change the Document Options for your Inventor part template (standard.ipt) every new part you create will use Radians as the default angular measurement.

Autodesk Inventor: Quick Tip - Tolerances Part 3

Just like my favourite movie Back to the Future, all good things come in threes and here's the third and final installment of using tolerances in your 3D models with Autodesk Inventor.

So far we've had a look at adding tolerances to 3D parts so that the data can be re-used in the associative 2D drawings, but also how we can re-evaluate the 3D model based on the upper, lower and median tolerance to check things like fit and function.

This final part of the trilogy looks at how we can set general tolerance values to comply with company\project standards.

Many engineers and manufacturers work to general tolerances that are set either in company standards or at the beginning of a project. These tolerances are applied to all dimensions so that manufacturing are using the same tolerance values across all parts and features. Autodesk Inventor allows users to set general tolerances within the Document Settings and apply these standard values to the 3D model automatically.

First, go to the Document Settings option on the Tools ribbon...

And then from there just select the Default Tolerance tab....

The Document Settings dialogue allows you set default settings for the current part (.IPT) document you are in. The General Tolerance tab allows you to apply the tolerance values for each precision as well as export these values to your document iProperties.

When you add a tick in the Use Standard Tolerancing Values option you will be able to add Linear and Angular tolerance values against a precision. Just select a precision from the Precision drop list and then type in the tolerance value you wish to apply to any dimensions using that precision:

You don't have to apply a tolerance for all precision values, you can add just the ones you use.

If you add a tick in the Export Standard Tolerance Values option, the values you input as standard tolerances will be exported to the iProperties of the part file you are in. Keep reading to see how we can use these values in our drawing:

Once the standard tolerance values have been set you can use them in your 2D sketches to apply the tolerance value using the Tolerance... option in the Edit Dimension tool. Just select the precision and make sure the type is set to default and the standard tolerance for that precision will be applied:

You can see in the example above that by selecting a Precision of 0. and having the Type set to Default a tolerance of 2.5mm (upper & lower) has been automatically applied.

In the example below I have chosen a Precision of 0.1 meaning the tolerance has been set automatically to 0.25mm:

So now we have applied the tolerances to our 3D part, when we come to create the detail drawings how can we make sure that all of the tolerance values are automatically annotated?

The fact that we selected to Export Standard Tolerance Values so that they are available in the part iProperties means we can re-use those values in the drawing. The way I do this is to create a Sketch Block which contains the following:

The <ParLinTol0> values are text values that are linked to the part document meaning the value will be pulled from the part documents iProperties. So whatever the standard tolerance values are in the part document, they will be automatically shown on the drawing. Having this as a sketch block in the 2D drawing means I can add it to any drawing, at any time to annotate the values automatically:

Adding the standard tolerance values and sketch block to your part template(s) will mean that every part and drawing you create will already contain the standard tolerance values and sketch blocks you need saving you having to apply them every time.    

Autodesk Inventor: Quick Tip - Tolerances Part 2

On Wednesday I posted an Autodesk Inventor Quick Tip all about adding tolerances to your 3D parts so that you can automatically annotate your 2D drawings with the tolerance data. If you update the dimensions and tolerances in the 3D model - the tolerance data automatically updates on the drawing! Today I'm going focus on using the tolerance data in the 3D part(s) to re-evaluate the parts and see how manufacturing at the upper\lower tolerance can affect fit and function.

Using the same part we used on Wednesday I have edited the tolerance values in the 2D sketch so that we can see the effect of re-evaluating the model using the tools in Autodesk Inventor...

To update the 3D part so that it using the tolerance values to size the part, all you need to do is open the Parameters dialogue.

The parameters dialogue includes a Tol. column which as you see above shows a yellow circle for all dimensions. This means all dimensions are currently set to their nominal value e.g. the dimension value you entered into the sketch. However, we can re-valuate all the dimensions in one go using the four options in the Reset Tolerance tools (from left to right):

• Upper Tolerance
• Median Tolerance
• Nominal Tolerance
• Lower Tolerance

Clicking on one of the options will set all of the dimensions in the parameters dialogue to the tolerance value:

You can see in the example above, by clicking on the Upper Tolerance option, the Tol. column now shows all the dimensions with a + meaning they are all now at their upper tolerance value. The highlighted values are the two dimensions I've applied tolerances to and if you look at the model value you can see that they are different to the nominal value - they now include the addition of the upper tolerance values I applied in the 2D sketch.

If I select the Lower Tolerance option, you can see in the screen shot below, all of the dimension values update to the lower tolerance values I applied in the 2D sketch:

So now we have reset all of the dimensions to the lower tolerance value I selected in the Parameters dialogue, lets see how that effects the 3D part:

You can see from the screen shot above the model is now smaller, if I measure the width of the part I can see that it is 223mm rather than the 225mm I applied in the sketch. This is because I have select to re-evaluate this model at the lower tolerance so 2mm has been taken off the width.

When we see the drawing detail of this, Autodesk Inventor shows in the annotation that the dimension has been re-evaluated by adding an underline to any dimension that has an upper, lower or median tolerance applied in the 3D part:

We don't have to apply tolerances to all dimensions at once, we can selectively choose which dimensions we wish to re-evaluate by selecting the tolerance from the drop list in the parameters dialogue. This allows us to mix upper, lower, median and nominal in different sketches:

Having 3D parts in an assembly that have been re-valuated at different tolerances gives us the ability to check for clashes and interference so we can see exactly how components will behave with each other when manufactured at different tolerances:

Thanks to Mike Watkins for the prompt to put these two posts together.

Autodesk Inventor: Quick Tip - Tolerances

When manufacturing parts it is common practice to add tolerances to dimensions to aid manufacturing. In some cases an overall or general tolerance is shown the drawing being used for manufacture, and in other cases individual tolerances are applied to dimensions on the drawing.

Autodesk Inventor allows users to apply tolerance values to dimensions in the 3D part model which can be then be used to automatically annotate the associative 2D drawing but can also be used to show the 3D model at the different tolerance sizes to check for fit and function.

First, we're going to have a look at adding tolerance values to our 3D part model and using them in the 2D drawing for manufacturing.

Step 1: Adding tolerance values is really easy, just click on the > arrow on the end of the Edit Dimension box and select Tolerance from the list...

Step 2: The Tolerance dialogue allows you to select the type of tolerance you wish to add, as well as well as set the Precision and set the Evaluated Size (we'll talk more about that another time)...

Step 3: Select from the Tolerance Type list, the type of tolerance you would like to apply...

I found the definitions for each of the tolerance types on the Autodesk Wiki....

Default
Used if you do not specify a tolerance type.

Symmetric
Specifies the same value at the upper and lower tolerance range.

Deviation
Specifies a different value at the upper and lower tolerance range.

Limits - Stacked
Displays the maximum and minimum tolerance values in a stack.

Limits - Linear
Displays minimum values and maximum values side by side separated by a hyphen.

MAX
Displayed as a label on the maximum tolerance value. The upper tolerance is zero and is disabled; the lower tolerance level is any number equal to or greater than zero.

MIN
Displayed as a label on the minimum tolerance value. The lower tolerance is zero and is disabled. The upper tolerance is zero and is disabled; the upper tolerance level is any number equal to or greater than zero.

Limits and Fits
Used to show tolerances on shafts and holes in addition to tolerances for the part. Nomenclature and tolerances are specified by the standard selected (such as ANSI or ISO) when Autodesk Inventor was installed. Limits are the tolerances for a part; fits are the pair of limits for a pair of mated parts. Stacked and Linear options are available. The Show Size Limits option displays the tolerance limits in parentheses. The Show Tolerances option displays values in parentheses with a plus and minus to indicate the upper and lower tolerances.

Step 5: Once you've applied the tolerance value it will be shown on the dimension in your 2D sketch...

NB: If you can't see the tolerance value like it shown above it is most likely due to the Dimension Display settings. Just right mouse click in the sketch and select Dimension Display from the list and make sure there is a tick next to where it says Tolerance.

Step 6: Create a 2D drawing view of the part as a DWG or an IDW, right mouse click over the view and select Retrieve Dimensions...

Step 7: Select the model dimensions you wish to show on the drawing view from the preview and when they are applied to the view you will see that the tolerance values you applied in the 3D model are automatically annotated to the drawings on the 2D drawing...

The tolerances are associative to the data in the 3D model meaning a change to the values in the 3D part will automatically update on the 2D drawing.

Next time, we'll have a look at how we can use the tolerance tool to automatically re-model that part based on the tolerance values.

Autodesk Inventor: Quick Tip - Axis Normal to Surface

Here we go, another quick Autodesk Inventor tip - this time it's how to use in-line work features to create geometry that stays normal to a face or surface.

It's pretty straight forward, and one of the tips to use for this to save some time is use in-line work features, which basically means you can create multiple work features at the same time.

If you want to create a work point but you need a work axis first, just select Work Point and then right mouse click where you will be given the option to create a Work Axis and Work Plane first. Once you've created the in-line work axis, select the final piece of geometry for the work point and in one function you've created everything you need.

Have a watch of this in action and how it can be used to create geometry that always stays normal to a face or surface

Autodesk Inventor: Quick Tip - Keeping up with Content

There is so much useful & informative content on-line about software such as Autodesk Inventor, Vault, AutoCAD etc that sometimes it can be difficult trying to keep up!

One tip that I use to make sure I stay up to date but don't have to spend hours and hours trawling around the web is to add the RSS feeds of the sites & blogs I visit regularly to my Autodesk Inventor Communication Centre.

This makes sure that all of that useful information, updates, tips, tricks etc are automatically delivered to my Autodesk Inventor user interface whilst I am working. You cad add any RSS feed so if you follow a particular Twitter user that shares good tips, or maybe you read a blog regularly (this one for example) you just have to copy the URL of the RSS feed and paste it into your Autodesk Inventor Communication Centre and the content will be automatically delivered to your application. You can also build your own RSS feed from the Autodesk website based on what you are interested in knowing. Use the link below to build your own custom RSS feed:

http://usa.autodesk.com/adsk/servlet/index?id=9813092&siteID=123112

(I created a custom RSS feed that tells me each time a hotfix or update is released for Autodesk Inventor and added to the Updates & Downloads page)

Here's a quick video showing how you add RSS feeds to your Autodesk Inventor application.....

Autodesk Inventor: Quick Tip - Section View Alignment

Another quick Autodesk Inventor 2012 tip for you that I used earlier today whilst documenting the design of a casting I'm working on.

Section views are so valuable so that design engineers can see whats going on inside a design but also so that those in the shop floor manufacturing the component can also see whats going on.

Autodesk Inventor allows a user to create a section view of the 3D part and\or assembly as well as create a section view for the 2D detail drawing. Now when you create a section view in a drawing, it is automatically projected either vertically or horizontally. But what do you do if there isn't enough space on the drawing sheet to place it directly above or to the side of the parent view?

This quick tip shows how you can quick de-align the view during the creation process....

Autodesk Inventor: Quick Tip - Selection Filters

Sorry......I've been a bit quiet posting new blogs and YouTube videos lately! With the launch of the new Autodesk 2012 Digital Prototyping Solutions it's been a hectic couple of months with a lot of travel but it's been great meeting designers, engineers and manufacturers to talk about how the new Autodesk Suites will help them.

One of my favourite tips when using Autodesk Inventor is using the Shift + right-mouse button to access the list of selection filters. It's a great way to select exactly what you want quickly and easily directly in the geometry window without having to look in the model browser and activate parts & sub-assemblies.

I use this work flow a lot when I want to change a feature of a component that is buried deep in the model browser amongst all of the parts, sub-assemblies, work features etc. Just hold the shift key on the keyboard and at the same time click the right-mouse button. You'll get a list of all of the selection filters and options - the one we want is Feature Priority. Just select it from the list as as you move your mouse around the geometry features are highlighted and can be selected - regardless of what level they are at in the model tree.

The selection filter shortcut also works in the drawings environment where you can select parts, features and also quickly select annotations such as Model Dimensions or Overridden Dimensions. You can use the Part Priority in a drawing to toggle the visibility of a part in an assembly drawing!

Here's a quick video of this in action......

I've got a list of more Quick Tips that I'll be posting over the coming weeks and months so make sure you vist back.

Guest Post: Autodesk Inventor Hole & Thread Data

This is the first in a number of guest posts on the Autodesk MFG Blog from users with some great tips & tricks to share. If you want to share your tips & tricks, click here.....

Today UK based Autodesk Inventor user Paul Munford shares his tip on configuring Autodesk Inventors hole and thread data. Take it away Paul.....

Autodesk Inventor provides great support for many local, national and international drawing standards. How can you put your standard at the top of the Threads and Clearance lists?

If you are living and working in Northern Europe, it is likely that you are using the ISO standard, or your own National or Local standard. If you have installed multiple standards with Autodesk Inventor, you may find that the ANSI standard is at the top of the list!

You can easily put the ISO (or your own) standard at the top of the list used by the Hole tool and the Thread tool and save yourself countless picks and clicks.

There are five steps:

• You will need to close Inventor down.
• You will need to find which copy of the Thread.xls and Clearance.xls your current project is using.
• You will need to create a back up copy of these files.
• You will need to edit these files.
• You will need to start Inventor up to test your changes.

Finding your Thread and clearance file path:

Inventor uses two Excel spreadsheet files to contain all the data required by the Hole tool and the Thread tool.

The Thread.xls file contains all the data for internal and external threads, and the Clearance.xls file contains all the data for unthreaded holes.

You can find both of these files in the Design Data folder, usually within your documents path:

C:\Users\Public\Documents\Autodesk\Inventor 2011\Design Data

Tip: If you don't find your thread and clearance xls files in this folder, check the Libraries path in your project filefor the location.

Edit the Thread file

Make sure that Inventor is shut down and that you have backed up the thread.xls file before you go tinkering!

Open the Thread.xls file in Excel and check out the value of the cell ‘D1’ on any tab. As you can see, cell D1 contains a value for ‘Sort order’. By changing this value you can re-sort the order in which Inventor will display the information in the Hole and thread tools.

In the screen shot below, you can see that I have set the value of cell D1 to ‘sort order - 1’ on the ISO metric profile tab to bring this to the top of the list.

I then edited the value of D1 on the ANSI tab to make sure that there was no conflict in values.

Tip: Make sure that Excel saves the file as an XLS file – not the newer XLSx format.

Tip: Don’t forget to make sure that the cell D1 on each sheet contains a unique value!

Edit the Clearance file

Make sure that Inventor is shut down and that you have backed up the clerance.xls file before you go tinkering!

Editing the Clerance.xls file is very similar, but this time we need to edit the value of cell B1. Once again I have edited the values in the ISO sheet and the ANSI sheet to make sure that there is no conflict.

Tip: Make sure that Excel saves the file as an XLS file – not the newer XLSx format.

Tip: Don’t forget to make sure that the cell B1 on each sheet contains a unique value!

Restart Inventor and check it out!

Start up Inventor, try out a hole or thread and check it out!

The updated hole tool:

  

The updated thread tool:

Job Done!

Making this quick edit to your Threads and Clearances data files will save you having to select your preferred standard every time you use the Hole and Thread tools

About the CAD Setter Out.

Paul Munford is a Joinery draughtsman (a ‘Setter Out’) for Beck Interiors; a UK based international Interior Fit out contactor which specializes in Museum Interiors.

Paul uses AutoCAD and Autodesk Inventor to create manufacturing ‘Workshop’ drawings day in – day out.

In his spare time Paul writes the ‘CAD Setter Out’ Blog and wishes he got out more.

Quick Inventor Tip - Projected Sketch Geometry

If you're working in an Autodesk Inventor assembly and you're working top down, it's likely that you will be projecting sketch geometry from one part to another.

When using the Project Geometry tool in a 2D sketch from one part to another, depending on how you have your Application Options set, the geometry you project will be associatively linked to the source. This means if the source changes, the projected geometry will also change. This can save you a lot of time updating and positioning.

However, if you just want to project geometry so that it isn't associative, there is a quick tip that can help.

Just hold down the Ctrl key on the keyboard when you select the geometry to project and you will end up with the geometry projected but not associative.

This shows how associative projected geometry is shown within the model browser by projecting (without holding the Ctrl key):

This shows how non-associative projected geometry is shown within the model browser by projecting (holding the Ctrl key):

If you find yourself using this tip regularly as you don't want to have projected sketch geometry associative, you can change your application options by taking the tick out of the Cross-Part Geometry Projection option: