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PTC Creo not retaining dimension values?

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Newbie

PTC Creo not retaining dimension values?

Hello,

Whenever I create a model, and add dimensions to it, PTC does not seem to save the exact value. For instance, I dimenesioned a hole to .375 inches. When I enter it, the dimension value changes to .38 . When I click on it to edit it again, it comes up .375 . This is normal, I know. The problem comes when I save the model and quit Creo. When I come back to the model, the dimension value read .38 inches, but when I click to edit it, it still comes up .38 inches. Creo seems round off the dimensions after I save the model and come back to it.

This is a very concerning issue that I can not figure out. I have to manually change all the dimesion values that go past three decimal places. Please advice me if you know what is going on. Thanks in advance!

4 REPLIES 4
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Re: PTC Creo not retaining dimension values?

This is not normal behavior. The only time I see this kind of rounding is when the value is used in a different dialog. I do find this behavior troubling when this does happened, but it does not happen when you create a feature with implicit dimensions.

To minimize input rounding, I always model with precision to 4 places (inch). I know I have to change each dimension in a drawing, but this is a good time to determine if I want 2 or 3 decimal places.

Also remember that by default, limit dimensions cause the nominal value to change. I don't like this and I set this in my config.pro: maintain_limit_tol_nominal yes < intuitive huh!

I remember in early Creo 1.0 F000 this seemed to be more prominent. As I progressed into Creo 2.0, rounding was only prominent in the ribbon dialogs where you could put a formula in, say 3/16 (.1875) and it would round to .188 if decimal was set to 3. And it would stay that value.

If you can upload a short video of your experience, and upload the file, we can duplicate your experience. If indeed it changes from the session version to the saved version, PTC will need to answer for that.

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Re: PTC Creo not retaining dimension values?

Here is an example of a "ribbon dim" change... compared to a section dim.

The .6667 was entered as 2/3. The value only takes on the value of the number of places designated.

Unlike the dimension added in a section, where the value 1/3 remains .33333333333333 and displays as .3333.

This really is a problem with me. Anytime I use a arithmetic operation for a value, I expect that value to remain to the maximum number of places without having to re-edit this value later. If I go in and change the properties of the extrude depth dimension, I can set it to 4 places, rounded, and use the same calculation of 2/3 and it remains .666666666667 and shows as .6667. Now when I edit this value in the graphics screen, the popup shows .666666666667 as it should have in the 1st place.

I have tried every way to change this to see if it changes after save. I cannot reproduce what you are saying.

Make sure that the properties of your dimensions are set to rounded. If not, it will change the dimension to the number of digits specified.

Example of Ribbon Dim...

ribbon_dim.png

Section Dim

section_dim.png

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Re: PTC Creo not retaining dimension values?

Thank you for your help. I had no idea that using an equation could result in these errors. I have since turned up the accuracy and changed the display dimensions to 4 digits. It has seemed to solve this issue, since now the dimensions stay the same after coming back to the file. Again, thank you for your quick reply!

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Re: PTC Creo not retaining dimension values?

Happy to help Mark. Welcome to the forum!

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