Override a dimension to create a Basic Dimension

[Anonymous]

Is there a way to override a dimension and have it shown as a GD&T Basic dimension. I can override a dimension with

the text option but not with a box around the letter. It sounds strange to do this but the letter represents a dimension in a

chart format that are Basic dimensions. Thanks

Randall

[Anonymous]

Let me offer a better explanation of what I am trying to do. I am placing a dimension on a part. I hide the dimension

and put a text letter, example A instead of the dimension. Now I want a box around the A representing a basic dimension.

Is that currently possible? After reading some of the posts on this subject, I am not too sure it can be done.

Thanks

Randall

[dave.anderson]

I can offer a few different ways of doing this, but you're correct. Once you've enabled the option to Hide Dimension Value, any associated tolerances (in this case the Basic value) are no longer applied so you will not be able to do this entirely from the Edit Dimension dialog box.

Here are some options that may work for you:

1) Use the Hide Dimension Value option and manually enter the text, then create a view related sketch and draw a rectangle around the text

2) Create a sketch symbol with a Prompted Entry value and a box around it and insert it where the Hidden Text would be. Insert it so it's attached to the dimension.

3) Insert a Datum Identifier where the Hidden Text would be. This can be attached to the dimension.

You may have to be creative with using spaces for Hidden Text would be to have the dimension line not overlap.

I hope this gives you some ideas.

[Anonymous]

Sure you can....

[Anonymous]

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@Anonymous wrote:

Sure you can....

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No Dennis, you can't. What the OP is trying to do has been a request for years.

[Anonymous]

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@Anonymous wrote:

Is that currently possible? After reading some of the posts on this subject, I am not too sure it can be done.

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The best solution I've seen is to override the dimension with a letter using the Text tab, then use a sketched symbol that is just a simple rectangle. Insert the symbol with a leader (not visible) so it "sticks" to the dimension.

[Anonymous]

Sorry, I missed the "Text Option" statement, but you can override with a different than default numeric value.

I gave up table driven parts years ago.... 

I agree that would be a nice option, however...

[Anonymous]

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@Anonymous wrote:

I gave up table driven parts years ago.... 

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You don't teach iParts? iPart drawings set with alpha character dims and a corresponding table are a very slick way to manage part families because it allows you to manage 1 drawing for many parts.

[Anonymous]

Yes, I teach iParts.

In over 40 years of working with table based drawings, I've seen way too many errors (and scrap) in reading dimensions from tables. It's so easy to drop down a line when there are numerous dimension columns.  Table drawings existed because drafters did not have to create a new drawing for each variation. With Inventor, that procedure is simple and automated.

I strictly teach  1 part = 1 file = 1 drawing file.  It's easy to substitute specific iPart members in an existing file.

If you want to do things the way they've been done for a hundred years, that's your choice.

[Anonymous]

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@Anonymous wrote:

In over 40 years of working with table based drawings, I've seen way too many errors (and scrap) in reading dimensions from tables. It's so easy to drop down a line when there are numerous dimension columns.  Table drawings existed because drafters did not have to create a new drawing for each variation. With Inventor, that procedure is simple and automated.

I strictly teach  1 part = 1 file = 1 drawing file.  It's easy to substitute specific iPart members in an existing file.

If you want to do things the way they've been done for a hundred years, that's your choice.

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Well when I have an iPart drawing that has over 6 dozen variations, and we implement an ECO that affects all of them, I'd prefer to manage one drawing to implement that change. Rather than putting in ECO's against almost 80 drawings. And in other cases when just one variation is revised we handle that in the table as well. It's a flexible and efficient system. And if it's been done for a hundred years, that's probably the reason.

There are a host of ways to protect against the risk that someone will read the wrong line in the table. And I've seen the same mistake you talking about happen as often when a drawing for each variation exists and has just one dimension that is different. It's easy for someone to miss that one change in those cases also. Further, in the modern age where so many part files are read into CNC, these table based drawings are often used more for reference, approval and checking the end product than for machining from.

We also like to use table based drawings for data sheets to be placed on the website. This is a far better way for us than creating one drawing for each variation and expecting a customer to download 6 dozen PDF files to find the size they need.

1 part = 1 file = 1 drawing file is a great method, and one I use and recommend using most of the time. But I'm not sure I agree with teaching "strictly" that method to the exclusion of all others, but of course as you said "that's your choice." 

[Anonymous]

I guess.... 🙂

Actually, I do discuss tabled drawings but include my caveat. Yes, there are situations where the old method may apply, such as in your case.

[Anonymous]

I figure out that it is easier to over write the std dim. to basi by clicking on the dimension you want to conver to basic or control with the dim control box, then rigth click, select properties, select text tab section, select frame text! (for mixed dimension styles, basic and std)