Units setting

[ptc-4696138]

I'm new to PTC/Creo ProE or whatever they call it now. I'm trying to set the units, and it looks like the default is 0.0012, and I can't seem to change it "globally", as everything is grayed out until I open a drawing. Do I have to set the units every time I start a drawing? Also, it looks like the minimum accuracy is 0.00001... this is not nearly as accurate as Inventor or SolidWorks. Is this correct?? Can I set the units to the maximum accuracy and have it open each new file at those units or do I have to set the units every time?

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[TomD.inPDX]

I don't think you are referring to units but instead "accuracy value".

It gets deeper than this and I find it most annoying.

There is "Relative Accuracy" and "Absolute Accuracy"

1st of all, you have to set allow_absolute_accuracy in config.pro. Next, you have to set the accuracy to Absolute in the dialog you found. You do not have access to this without the config setting.

The idea is that a big part shouldn't require a small dimension feature. This is the "relative" part of the thinking.

There are ramification both ways but in general, the default in Creo is insane. I often create sheetmetal parts with a thin veneer of silkscreen. I found I couldn't do this and asked the same questions you asked. This is what led me to understanding that out of the box, Creo is a PITA.

Now, in general, we all use template parts or in the old days, "start_parts" that have everything set to where you want them. This is one of those settings you just have to know but I would set config.pro to allow absolute accuracy by default. It doesn't change to that, but gives you the option in the appropriate setup dialog.

[ptc-4696138]

Where is the "config.pro" located, can I access it from Creo, or is it on the "C" drive and I have to open a file? If it can be done from Creo, I can do it, but I have to get I.T. if it's on the local drive. Thanx for your help. I have a short tolerance for software anyway, and I'm finding Creo to be... quirky....

[TomD.inPDX]

No problem. Yes, you can change this setting under File/Options/Configuration Editor.

Use the find button and search "absolute".

enable_absolute_accuracy needs to be changed to "yes" (set value).

Click add/change and close.

Click OK.

You will be asked if you want to save the config.pro file. You do not need to as the option will be saved with your file.

NEXT!

So a few words on config.pro

This file has 100's of options. Often, yes, enterprise settings try to control the defaults so not everyone has something different.

The way config.pro is read is one of two ways.

There is a default folder where Creo is started. If the config.pro file exists in that folder, it will read that file. If not, it will read the default in the Creo folder on your hard drive. If administrators are managing the config.pro file, you might drop them a note about this so they can change the default.

The second way to change config.pro wholesale is to import a saved config.pro file using the same dialog as above.

This is basic PTC Creo knowledge. Without it, you won't go far with Creo. In general, if admin takes care of it, put them on speed dial. Otherwise, you might start collecting links on how to make changes on the fly.

...next you will want to know about detail.dtl

[ptc-4696138]

oops... I poster just before I saw your reply. I'll look at it now. thanx

[ptc-4696138]

Oh, fer pity's sake... to quote the rant I use when Inventor starts playing up, "HOW do these people stay in BUSINESS????" I set the accuracy to "absolute", now instead of my accuracy being a ridiculous 0.0012, it's an absurd 0.086599076277. I can get closer than that with a YARDSTICK!!! How do I choke it into giving me a reasonable accuracy for a firm that models close-tolerance machined parts, say, 0.00000001 like Inventor will give me (for half the price)??????

[TomD.inPDX]

You set that value. I set it to .00005 and it regenrated although when I went too far, it said the range was quite a bit higher.

There are a few other settings you might check out.

I fully appreaciate your frustration.

[TomD.inPDX]

And before you get to this one...

SET THIS AT SOMETHING OTHER THAN DEFAULT!

[TomD.inPDX]

Indeed, I just tried this with a default part and setting and got the same values you did. This is because the default part, with no geometry is "HUGE" so the accuracy is limited.

Once I set the default_abs_accuracy to .000001, it allowed this value in the accuracy setting of the part.

I've worked in precision machining for the better part of a decade. Rarely do I need to go past 4 digits in inches. on occasion, I have to work in angstroms, but not for machining.

There is logic behind these settings but I find the defaults to be horridly restrictive. The idea is that using settings such as this will ease a lot of CPU cycles since Creo is still not multithreading. I suspect, however, that the defaults serves less than 10% of the user base. Everyone else has to learn this the hard way, like you did.

Hopefully you will get settled with Creo. I find this forum to be a valuable recourse when we get stuck on issues that seem "so simple"

[ptc-4696138]

I found the config.pro... actually 4 of them. Before I call I.T., can someone enlighten me as to which one contains teh secret formula for changing the "absolute accuracy" (with a name like that, it's gotta be a secret...)

[TomD.inPDX]

...and to "enable" absolute accuracy, you have to have a part or assembly open and go to file/prepare/model properties ...material/accuracy/change/ and select absolute where it says relative.

[ptc-4696138]

... good grief... this is ridiculous...now it's telling me .007 is the best it can do... it was .0012 BEFORE....

[TomD.inPDX]

see above