Dimensioning Chamfers

[ptc-2049565]

We're new at this! Can someone tell me how to place a drawing dimension for a chamfer so it displays something like .030 x 45°

Thanks in advance.

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[merrill.rosenow]

Hello Charles,

Whenever I am faced with a similar problem, I always use the same approach. If you know the dimension name of a specific dimension, you can reference it in your note. The dimension will then appear with the proper value in the note, and will also update when the dimension is changed. To do this:

- Open your model

- Right click, and select "Edit" for the related feature

- You will now see all of the related dimensions pop up on the screen and reference the model

- Left click to select the dimension you are looking for, then right click and go to "Properties"

- Open the "Dimension Text" tab at the top

- Near the bottom in the name field, you will see a value, d106 for example

- This is the name you are looking for

- Go into your drawing, and in the note you want the value you appear, type &d106

- When you complete the note, you will see in the place of &d106 that the value of the dimension appears

- You will have to add the º (degree) symbol manually since notes do not have the same properties as dimensions in the drawing (e.g. you cannot change the tolerance of a note, you'll have to put it in manually)

[JeffS.]

Why not set this up in the config.pro? The behavior of the note is
controlled with the command:

chamfer_45deg_dim_text asme/ansi

This will automatically set chamfer feature dimensions to display as
requested, possibly depending on the construction. Remember you will need
to create the chamfer as a D by angle type chamfer.

Regards,
Jeff

Jeff Schnellinger
Senior Mechanical Engineer
jeff.schnellinger@kistler.com

[JonathanHodgson]

If you've created the chamfer as an [Angle×D] type, it's actually slightly simpler (to my thinking):

In the drawing:

Show the chamfer length dimension
Right-click->Properties (or double-click) the dimension
and change to the Dimension Text tab
The text will be "@D"
As below, the name field will contain "d106" or similar
For [Angle×D] chamfers, the angle dimension is one number higher than the length, so:
Change the text to "@Dx&d107" (don't type the quotes!)
OK the Properties box.

With this technique, you should find that the ° (degrees) symbol is included automatically.

HTH,
Jonathan

[TimMcLellan]

A couple of more options:



You can add/change your config.pro file to include: chamfer_45deg_dim_text
iso/din

This option will produce the result 1.25 x45 º for your model and when
showing dims in the drawing.



However, if that is sill not exactly what you want you can (in the drawing)
select the chamfer dimension and choose ?properties? similar to Merrill?s
comments below. One minor change is while you are in the Dimension
Properties Dialog Box and under the TAB Properties go to the bottom left and
look for the option ?Chamfer style?. Using this option allows you to
switch/toggle the chamfer style to different options. You can always choose
?Customized? and then go to the Dimension Text TAB and tweak the text anyway
you want.



For example (using the config setting above):

Initial shown dimension looks like: 1.25 x45 º

Switching to Customized you can change it to: 1.25 X 45 º



Hope that helps,



Tim McLellan
Mobius Innovation and Development, Inc.