How to change the precision in the Evaluated Value of the Custom Property "Thickness" (sheet metal)

[bnemec]

I would like the Thickness property to Evaluate to three or four places. As it is now a part set to 12GA thickness will show 0.1 Which isn't much good. a 7GA part shows as 0.18 or 3/8 as 0.38

I would rather it resolve to the gage number from the GageTable.xls but we gave up on trying to get that to work.

Here's our GageTable, it's very elaborate.

And this is how the Thickness property evaluates for a 12GA part:

How the Sheet Metal feature settings are:

And How the print looks:

If someone could guide me to how to have the material custom property always evaluate to 4 places that would be nice.

If there's a straight forward, not house of cards, way to display the thickness as the gage number (or fraction on the thicker stuff) that would be better.

Thank you.

[HerrTick]

Displayed decimal places may be tied to your measuring tool precision or properties precision.

[HerrTick]

A roundabout way to get the precision the way you want might be to assign the Thickness value to a variable. (Old Pro/E trick.)

[bnemec]

A roundabout way to get the precision the way you want might be to assign the Thickness value to a variable. (Old Pro/E trick.)

Oh boy, another link in the chain. Coming from SE so users cannot figure out why they cannot directly pull model data from the drawing and why a custom property is needed in the model "expose" the model data. So now it would be Model Data -> Variable -> Custom Property -> $PRPSHEET

firing up some Fleetwood Mac now "The Chain"

[Glenn Schroeder]

I believe you could fix the issue by changing your Units to display the desired number of decimals (Tools > Options > Document Properties > Units); maybe on the Drawing, and maybe on the Part, and maybe both.

This may cause issues to dimensions in your drawing, but they could be overcome by going to the Other tab on the dimensions property manager, checking the box for "Override Units", and making your changes there.

You could select multiple dimensions and perform this operation on all of them at once, or even make this change once and save it as a Style, where it could be easily applied to existing and future dimensions.

[HerrTick]

I realized I gave up a long time ago on this issue. I reverted to a now longstanding habit of just showing thickness as a reference dimension.

[bnemec]

Displayed decimal places may be tied to your measuring tool precision or properties precision.

Checking Measuring tool in the Model:

As for "Properties Precision" I'm sorry but I'm not sure what you mean. Settings -> Document Properties?
Looks like it should always show 2 places.

unless... it is showing 2 places all the time but 12GA would be 0.10 Don't tell me it trims trailing zeros for me!?!? I've seen that somewhere...

I assume this only applies to drawings? But there's trailing zeros, and set to show:

[bnemec]

I believe you could fix the issue by changing your Units to display the desired number of decimals (Tools > Options > Document Properties > Units); maybe on the Drawing, and maybe on the Part, and maybe both.

The Doc Properties in the model will make it evaluate correctly there, but not on the drawing. So apparently $SPRPSHEET:"Thickness" on the drawing doesn't pull the "Evaluated Value" from the model.

If I set the "Units" precision to four places in the drawing Settings->Doc Properties then the note shows up as desired, regardless of what model is set to (in this case).

But now all the dimensions are four places just as you showed, but expecting users to manually set dimensions back to 2 places on every single new drawing is not going to work.

I'll look into Styles, haven't had opportunity or need to go there yet with SW Drawings.

It looks like I can set the dimensions back to two places in the Settings->Doc Properties->Drafting Standard->Dimensions to override what was set in Units.

So I think this is a solution, problem is it's another change to several templates and then the several thousand files out there started with wrong templates. Sure would have been nice to know what we were doing when we started and had all the templates and custom properties set correctly from the beginning. I'm beginning to wonder if this is worth a macro/api to update the Document properties when we change templates. The problems will lurk for years as these files won't show stuff correctly.

Thanks @Glenn Schroeder I didn't think check Units in custom properties, that changes so many things I was hoping there was a more tactical method.

[bnemec]

I realized I gave up a long time ago on this issue. I reverted to a now longstanding habit of just showing thickness as a reference dimension.

I remember reading that comment a lot a year or so ago when I was scouring the forum for how to get the gauge numbers to show up. I got lost in the round and round of properties and spread sheets and .....

I tried to just use dimension as you state, but getting kick back on that from Laser, they don't want to have to look all over the print for the thickness dimension when they're nesting.

About to just make it dumb text and have the designer keep it up to date; like AutoCAD days.

[Glenn Schroeder]

As you've probably figured out, overriding units can only be applied to actual dimensions, not to dimensions in notes that are linked to custom properties. I'm a big fan of Styles, but I understand your reluctance to depend on them to fix the problem.

I wish I had a better answer for you. Someone else might, but if so I'll be surprised. Pleasantly surprised, but still surprised.

[MJuric]

Thanks @Glenn Schroeder I didn't think check Units in custom properties, that changes so many things I was hoping there was a more tactical method.

I went thru this a while ago and I can't remember exactly what the solution was only that it was frustrating.

Along with Glenn's suggestion you will need to check every other place that there is a "Unit" change. Document properties for general units, dimensions, dimensions in the model, measuring and probably a half dozen other places I have forgot.

Why there isn't a single "Master Unit control" is beyond me. But in the end you can get what you want....you just have to hunt down and kill the right one.

What also makes almost no sense, at least to me at this moment, is how things are controlled. A note might be controlled by the dimension in the model but a dimension might be controlled by the document and so on.

[bnemec]

This all sounds to me like a house that has been built over several generations; from a one room shanty in the mid 1800s. a bed room here, a kitchen there, some wires over there, a bathroom up there, a basement down there a few more bed rooms here and there, more wires, more pipes.

I guess that's the problem we cannot see the end from the beginning and the requests of us fickle customers are just added on one block at a time. Frustrating for the customer, but it's almost our fault. However some careful planning and remodeling shouldn't be unfeasible; after all each release needs all templates updated, all files open/saved and we've come to expect APIs/addons to randomly not work after update. I digress.

[Merovingien]

the problem of "trailing zero" for properties, not working correctly in PRT.
i already saw another "dims" that don't follow the DOT unit setting...

we all know it's Bugidworks....

it seems "the trailling zero" is still a buggy feature in Bugiworks.

the three lines appear to be linked (parent-child) not independent....
to make it working, in PRT, you have to set it to "show"...
i created a dummy-extrude linked to the "thickness"
i set that dims to 3 digits
i call that dims in a property
i call that property in DRW

with that workarround, you avoid changing of unit in DRW.
but it's long workarround...

[MJuric]

the problem of "trailing zero" for properties, not working correctly in PRT.
i already saw another "dims" that don't follow the DOT unit setting...

we all know it's Bugidworks....

it seems "the trailling zero" is still a buggy feature in Bugiworks.

I had a discussion with my VAR on a trailing zero issue. It wouldn't display properly in either a BOM or Cutlist or something. End result, yep, "Apparently SW can't do that".

[Merovingien]

you can, with my (little long) workarround

the dummy-extrude is like a fake-feature, it's just to catch his dim.

it's a simple sketch with a circle, a square, or a triangle, whatever, fully constrained, or with a value 1 mm.
extrude-add in the main material, so it's invisible.
the extrude dim is set in panel-tree "same as sheet thickness"
and after, do the what i wrote in the picture...

but it's a long-workarround, not that great...

[bnemec]

you can, with my (little long) workarround

the dummy-extrude is like a fake-feature, it's just to catch his dim.

it's a simple sketch with a circle, a square, or a triangle, whatever, fully constrained, or with a value 1 mm.
extrude-add in the main material, so it's invisible.
the extrude dim is set in panel-tree "same as sheet thickness"
and after, do the what i wrote in the picture...

but it's a long-workarround, not that great...

That is a work around and agree with your descriptions of it ("not that great"). Thing is, as with many work arounds, is it's full of opportunities for error. While that work around may be the perfect fit for many, it sounds like manually adding the gauge number to the print is a more reliable work around for us.

Maybe someday my replacement, a new CAD/PDM Admin/.net person, can write us a "house SW add-in" that will take care of this and a growing list of other things Bugidworks "can do but..."