How to dimensions split edge chamfer with chamfer note

[Anonymous]

Hi everyone,

I'm trying to dimension a chamfer using the "chamfer note" option from Inventor, but since it is and angle profile that contains fillet, I am not able to obtain the accurate dimension. View from the top, the chamfer that I created in my 3D model creates a split edge when I import the view in the drawing, therefore giving me a wrong dimension. Any ideas on how to fix my problem ? (see image)

Thank you

[mcgyvr]

Dimension it without using the chamfer tool... or manually modify it.. 

Sadly it has these types of limitations as its looking at the actual line in the drawing and does not reference the parts features when it pulls its information..

[Anonymous]

There is no way to actually refer it to the model or a work around ? I don't want to manually modify it because I want the dimension to be linked to the model

[johnsonshiue]

Hi! I must not have followed the steps to reproduce it. I cannot seem to create such geometry with chamfer note like that. Could you share the example here?

Many thanks!

[mcgyvr]

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@Anonymous wrote:
There is no way to actually refer it to the model or a work around ? I don't want to manually modify it because I want the dimension to be linked to the model

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To avoid manual modification then you would need to do something like a angle and linear dimension to show the intent there..

The chamfer tool AFAIK cannot be used due to its limitations..

[mcgyvr]

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@johnsonshiue wrote:

Hi! I must not have followed the steps to reproduce it. I cannot seem to create such geometry with chamfer note like that. Could you share the example here?

Many thanks!

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@johnsonshiue Johnson it looks like the radius on the front part is not tangent to the front surface so that allows the front edge to be selected using the chamfer tool...

This is another limitation of Inventor thats been around for YEARS and needs to be addressed.. 

Show support for fixing it here..

https://forums.autodesk.com/t5/inventor-ideas/improve-chamfer-note-drawing-tool/idi-p/5031524

[Anonymous]

https://drive.google.com/open?id=16CROgxC6MGTR_l1nU4tUvieT3RZZ61pY Here is the model

[kelly.young]

Hello @Anonymous I see that you are visiting as a new member to the Inventor Forum.
Welcome to the Autodesk Community!

Make sure to vote up the idea, but the only workaround I know of in that situation is to change the Chamfer to Distance and Angle so it creates a dimension for the 45° (if it is always going to be 45° you can do just by distance). 

Within the drawing you can then link to the dimensions and have them change parametrically with whatever new value the chamfer is changed to. 

Hope that helps!

Please select the Accept as Solution button if a post solves your issue or answers your question.

[Anonymous]

Hi Kelly, thanks for your reply.

I have already did this but the reason why I posted here for an other possibility is because with this method, I am not able to display the dimensions as fractional values (unless there is a way to do so that I am not aware of). Let's say that my chamfer dimensions are 1.625 X 45°, I want the value to be displayed as 1'' 5/8 X 45° (for manufacturing purposes). Is there a way to do it ? Also, wouldn't it be possible to be able to select a different edge ? For example, when you are in the 3D model environment, if you stand still on a line and wait for a bit a drop down menu appears, giving you the possibility to select an other edge/face/axis. That would be helpful if the same thing would occur in the drawing environment. Where can I propose this idea for future version ?

thank you 

[kelly.young · Accepted solution]

@Anonymous if you want to have it be fractional it is possible, just a few more steps.

• Access the Parameters
• First, check option for Export *@mcgyvr nice catch on the necessary order*
• RMB on the dimension value > Custom Property Format...
• Change it to Fractional

• Create a Leader Text
• Find Type > Custom Properties - Model
• Click the Add Text Parameter button to populate the value into the text
• You can then link the angle through the typical Add Parameter mapping as well

You can post at Inventor Ideas if you have things you would like to suggest. 

Hope that gets you going!

Please select the Accept as Solution button if a post solves your issue or answers your question.

[mcgyvr]

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@kelly.young wrote:

@Anonymous if you want to have it be fractional it is possible, just a few more steps.

• Access the Parameters
• RMB on the dimension value > Custom Property Format...
• Change it to Fractional
• Check option for Export

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@kelly.young "close" ..

You need to click the check box in the "Export" column first THEN you can RMB and chose "Custom Property Format"..

Until you export its custom format is not an available RMB option..

[Anonymous]

Hi Kelly,

is there a way to save this note somewhere so I wouldn't have to recreate the leader text note every time ?

Thank you

[kelly.young]

@Anonymous the only thing I can think of is to create an Add Text User Parameter with the suffix you want, for example: °CHAMFER

Then Add from the User Parameter section of the Format Text box. 

 

Hope that helps!

Please select the Accept as Solution button if a post solves your issue or answers your question.

[tleonardi2GPP2]

I know this is an old questions, but I thought I would share my work around for this. Add a sketch to the view you are trying to dimension. Add a sketch line from end point to end point of the chamfer. Finish the sketch and then you should be able to add a chamfer dimension with the sketch line which will show the total length of the chamfer. 

[Frank.HallWQLC5]

Thank you @tleonardi2GPP2, this is a great workaround!

[ampster40]

When the chamfer note does not work, it's by far easier to skip it and just place a couple dims manually.

By the time you get done adding a sketch on top of your view in the drawing (which does not always follow suit if the model changes) you've spent more time than it's worth to detail a simple chamfer.

[Frank.HallWQLC5]

There is nothing to be gained by arguing the point back n forth @ampster40. It took a few seconds to project the geometry and draw a line, and then the Chamfer annotation works as intended. I simply wanted to express my gratitude to @tleonardi2GPP2 for taking the time to post, what I consider to be, the winning solution.

[ampster40]

If you want to consider this arguing by all means.  But that is not what I am doing.

I am providing over 20 years experience using this software in plain simple words.

I am warning you to be careful about depending on sketches you take extra time to create on top of views because they do not always behave when a model changes, thus taking yet more time to fix some later that could have been ignored.

If it works for you great.  

0.02 cents worth of being there/done that.

Enjoy!