How to change x.x/x.xx/x.xxx etc in 3d space? lower right corners of screen

[dunebuggyjay]

Hi Guys,

How do I change these values? I've seen a post saying its Linear_tol, but this doesnt seem to change anything.

now that we are testing out MBD, I'm noticing that in 3d these are not what I want shown for tolerances.

I want it to match my 2d drawings as:

.xxxx =+-.0005

.xxx = +-.001

.xx = +-.005

.x = +-.01

This is what Ive tried added to my config,pro with no luck in changing this. Im assuming my formatting on the config is not correct?

[MartinHanak]

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@dunebuggyjay wrote:

Hi Guys,

How do I change these values? I've seen a post saying its Linear_tol, but this doesnt seem to change anything.

now that we are testing out MBD, I'm noticing that in 3d these are not what I want shown for tolerances.

I want it to match my 2d drawings as:

.xxxx =+-.0005

.xxx = +-.001

.xx = +-.005

.x = +-.01

This is what Ive tried added to my config,pro with no luck in changing this. Im assuming my formatting on the config is not correct?

---

Hi,

contents of bottom right corner is hardcoded, you cannot change it. You can verify this information with PTC Support.

[dunebuggyjay]

Is there a way to turn these off then?

I don't want someone looking at my MBD models and thinking this is the tolerance I want. 

[MartinHanak]

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@dunebuggyjay wrote:

Is there a way to turn these off then?

I don't want someone looking at my MBD models and thinking this is the tolerance I want. 

---

Hi,

I tested different Creo versions. Starting from Creo 6.0 bottom right corner is empty. Up to Creo 5.0 bottom right corner contain tolerance information which is hardcoded and cannot be hidden.

[dunebuggyjay]

After some testing, The display on the bottom right corner of the screen is on and off by the config Tol_Display in the config.pro

But It needs to be on for me to put tolerances on my MBD dimensions. if its turned off, It wont allow me to add tolerances to my dimensions.

I'm using Creo 7.0.12.0

Ill make a ticket

Jay

[StephenW]

Just remember, tol_display in the config.pro is ONLY set on your computer, so if someone else opens your model and they have tol_display set to yes, it will display the tolerance block on screen.

[StephenW]

There is an option to turn them off, both in the config.pro and the drawing detail options, but it turns off tolerances completely, even on the dimensions.

Tol_display NO 

(same option, both in the drawing detail options and config.pro)

And then the config.pro option only sets your session of creo, not your model.

The drawing detail option turns it off all tolerances for that drawing..

It's not what you want by any means, it turns off all tolerances, not just the screen tolerance display.

After setting your linear tol setting, did you try making a new feature so that new dimensions are created, I think they will be created with the updated tolerances. Again, not really what you wanted.

[dunebuggyjay]

I did try making new dimensions with my linear tol settings in the config, It Didn't make any difference to anything.

If Tol_Display is set to NO, I cannot add tolerances to my dims. If set to YES it shows the same (wrong..or at least, not what i want) on the bottom right side of the screen, 

[StephenW]

I think you should open a PTC support ticket to get good info. I know I'm guessing.

My last guess is when a part is created or when the start part was created, maybe the tolerances are set then...I didn't test it and it really is just a guess. Honestly, if this was the case, I would expect it to be in the part detail options settings, but it isn't, so I suspect I am dead wrong.

[pausob]

The linear_tol settings from your config.pro - these define the tolerances in a brand new, empty part.  And one that is set for the ANSI/ASME tolerancing standard.

AFAIK, there is no way to change these values once you create a model.

So if you are using a "template" part when starting a new part, then you are stuck with whatever settings the maker was using when creating that template.

Note that this schedule of tolerance as a function of # of decimal places isn't shown if you switch to the ISO/DIN tolerancing standard:

also, I think your linear_tol settings that match your drawing standard should be:

linear_tol 1 0.01 2

linear_tol 2 0.005 3

linear_tol 3 0.001 3

linear_tol 4 0.0005 4

which shows up as:

on my screen.