Changing Parameter Property Format Default Values

[Anonymous]

Is there a way to change the default properties of the parameters without changing the units of the part model?

We model at least 99% of our parts with metric units because almost all of our customers' prints are in metric.  Then we put a parts list on each part drawing with the outer dimensions for our suppliers in inches because our suppliers are all American supplying SAE material.  For every part we have to go in to Parameters, choose the dimensions to export and use "Custom Property Format" for the outer dimensions, changing each from mm to inches, decimal to fractional and the precision to 1/32".  It would be very nice to not have to go in and change those options with every part we model.

[kelly.young]

Hello @Anonymous this might help you out.

Setup a User Parameter to the mm dimension and make it set to inch with Fractional Format.

Access iProperties > Custom to set the property to be brought into the Parts List.

Bring into the Parts List > Column Chooser, setup a New Property as the User Parameter name. 

That gets you the value as fractional inches without having to set up a new style and is linked to the mm dimension.

Hope that helps!

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[Anonymous]

I went through and added a new custom property and set its units to in.  How we include the part dimensions is to add the dimensions to the property by creating a custom iproperty in the part and define it as MATLDESCRIP = <d5> x <d4> x <d3>, for example, so that it pulls in the dimensions from the part and in theory keeps them current- if changes are made to the base dimensions of the part anyway.

When I pulled the dimensions into the new iProperty set with in units and not mm, the dimensions still came in with the units in mm ( it looks like because the individual dimensions had not been set to the custom format).

kelly.young has embedded your image for clarity.

[kelly.young]

@Anonymous can you go into Parameters and set a User Parameter for each: 

Then use them in your expression:

MATLDESCRIP = <d5in> x <d4in> x <d3in>

Does that work?

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[Anonymous]

Unfortunately no- it doesn't insert values because what is in the < > doesn't then match the exported parameter.

[kelly.young]

@Anonymous here is a screencast showing how I got it to work, I'm guessing that in Parameters the User Parameter Units weren't changed?

Forgot to show in Parameters if you RMB on a User Parameter > Custom Property Format... you can set Format > Fractional and Precision > 1/32.

Hope that makes a bit more sense!

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[Anonymous]

I see how you made that work with the d3in as an added parameter- I guess  I missed that step somehow before the screencast.  

I can add the d3in into parameters but I can't tie it in to my template  without adding geometry.

I appreciate your time in this- I will think on a way to try and get the double stack parameter to work.  I could just make myself a template with a block already in it and just adjust the sketch and extrusion dimensions rather than creating it from scratch.  In that case I don't think I would need to even double up- I could just set the original parameters with the Custom Property Format that I need.  Seems like sort of a silly workaround bu tI suppose it will work.

kelly.young has embedded your image for clarity.

[kelly.young]

@Anonymous it doesn't appear that the d3 dimension is listed in the Model Parameters, which is why it shows up red.

Are you trying to reference it within in an assembly?

If so, you have to Link wherever the d3 dimension is being defined, so whatever part it is coming from.

You can also use Derive to bring in reference dimensions, make sure the sketch that holds the dimension is visible so it can be selected.

Hope that makes sense, depending on how sensitive the parts are, if you can attach using Pack & Go as .zip that would be helpful.

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[johnsonshiue]

Hi! Could you attach the part of interest here also? I think you need to change the Custom Parameter Format within Parameters table. I don't think you can make such change to a custom iProperty with an expression. The expression is treated like a text. If you want to show inches, you need to set Custom Parameter Format like Kelly showed earlier.

Many thanks!

[Anonymous]

We can modify the parameters on each part individually, which is what we do now.  My issue is doing it every time, so I'm trying to make changes to the default formats of the parameters (in the template file) without part geometry in the part.

I was able to set up a part with a box in it and edit the format of the parameters and I will just use it as my starting point- it doesn't look like right now it is possible to change the defaults.

[kelly.young]

@Anonymous just a thought, would showing dual dimensions on the drawing ~ 2.00mm [.079 in] ~ be sufficient?

Or just switching the Annotation Format from mm to inch?

If you need it to be pulled into the Parts List there has to be some connection to the dimensions. Creating the F/X expression doesn't allow for Apply Units Formatting as it causes an Incompatible Units Error due to the "x" separator being a text character and not a number.

If you create an individual Column for each dimension you could simply just Apply Units Formatting and change the Units to inch.

I still think you can get it to work but will require a bit of setup to create the User Parameters for each part as it occurs and then set the Custom iProperties expression.

The template might be able to be setup to call the MATLDESCRIP but would have to make sure it was being called properly.

Hope that helps.

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[Anonymous]

We do use display dual units already... unfortunately for some strange reason it is insisted that we have the part's outer dimensions in a parts list, even for the single parts.  I guess our suppliers use it to base pricing on the outer dimensions and we give them the parts list instead of them having to search the print.

Our current process is to model the part, go in to Parameters, select the appropriate dimensions for export, select the Custom Property Format for the exported parameters, and type in a custom material description, ie. =<d6> x <d5> x <d4>.

The slight help that I had applied previously to the template everyone uses was to go ahead and put in our custom iProperty "MAT'L DESCRIP." and set it equal to "=<d6> x <d5> x <d4>" so that if you started the part with a box and dimensioned the long edge first, short side and typed in a dimension for the extrusion depth and chose those three dimesions for export it would come into the custom properties.  However, we still have to go into Parameters every time, check them for export and change the properties from mm to in., fractional and apply to existing comparable parameters.

The closest solution I can come up with is to create a template for a box and a cylinder, export the dimensions and customize the format and just modify the original sketch and extrusion values.  Because they are saved as templates it prompts for a new save name so that works out ok.

[kelly.young]

@Anonymous  It sounded like you were getting close, were you able to find a good workflow for getting the units into the parts list?

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[Anonymous]

I think that using the Box and Cylinder part templates is as close as I am going to be able to get for now- it works ok.