Dimension display (@D and @S)

[Chris3]

It does not appear that you can show an @S (symbol) in one place and then an @D in another place on the same drawing.

I have a family table of a part and I am creating a table showing all of the varied dimensions for the family table. I want to show the @S for the generic in the header of the table and then the @D for all of the instances. When I flip one and then do a re-gen however it changes the others.

I called PTC and they suggested I write a relation to copy the dimension value into another parameter and then call that out in the table (ie Table_A = A). Doing that prevents me from showing the tolerances though. Unfortunately it looks like you can't call out the dimension tolerance variable (ie tp0 and tm0) on a drawing like you can a dimension (&tp0 doesn't work).

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[Chris3]

I just realized that I can create a relation to copy the tolerance too (ie Table_A_Upper_Tolerance = tp0). I am going to do this unless I hear something better.

[JonathanHodgson]

It sounds like you're trying to have the same dimension show as both @S and @D - which you clearly can't do, because editing either instance of the dimension edits the same dimension.

Perhaps you could use the shown dimension as @S for the generic, and use created dimensions for the instances?

[Chris3]

I am trying to do something similar to what is shown below. I would have thought that I could show @S for the generic and @D for the instances since the instances are separate parts with their own dimensions but apparently this is not the case. I suppose I could use created dimensions for the instances, but that seems like more work and not as robust.

PTC suggested that I just manually type in the symbol names which rubs me the wrong way given that their name is parametric technology corporation and there is nothing parametric about manually entering the names in. My solution of using relations while certainly not ideal works and it keeps everything parametric.

[rcrerar]

Hi,

I think that what you are trying to do is fairly straight forward. Your drawing view will display the dimensions for arguments sake the length of the screw at 50.0mm, you want this to show 'L' or length so change the name of the dimension from d26 for example to L. then go to the display tab and enter as @s this will display L instead of 50.0

You will also see this in your models family table where the header has the original d26 and L to give you a clue as to what the column is displaying.

The harder part is probably where you need to learn how to report in repeat regions. Assuming you know very little about this I will try to give you a coincise idea of how to execute this. If you know more then I apologise in advance if it seems patronising.

Create a 2x2 table. You will need to define a Two-D repeat region. the first region will be the horizontal one. Click on repeat region/ add/two-D choose the first cell as row 2 column 1, the second cell will be row 2 column 2. then choose the vertical region row 1 column 2 and the second cell of that is row 2 column 2.

You then need to add the report parameters to drive the content. I have attached a screen shot of the content as it's a little too complicated to describe it all in one go. Note the 3 cells that are populated are the ones you defined in the Two-D repeat region.

If you've done this correctly the labels will be as you want and the values will be correct too all with nicely defined part numbers down the left.

[Chris3]

Yes, I know how to create a repeat region. The problem with a 2D repeat region is that you can't add additional text / parameters into the repeat region. 2D repeat regions also don't support tolerance display (which I need).

[rcrerar]

Hi Chris,

You could add header boxes before you define the two-d repeat region and I would consider creating an upper and lower tolerance parameter then adding these to the family table that way they can be reported on. You also should be able (i think) to add the relation to make the tolerances equal the parameter.

[Chris3]

Yeah that's exactly what I am doing (see second post). You don't need a repeat region if you are going to go down that path. You can pull in the &d0 dimensions into the table along with whatever parameters and text you want. This is the solution I have now.

[Kevin]

It may not give the form you want but you can directly report the plus and minus tolerance values but not the dimension limit values. You add the tp and tm values to the family table by specifying OTHER in the selection radios.If you have already renamed the dimension you still need to specify the dimension number for the tp or tm value to be added to the table.