Questions regarding Dual Dimensioning on Weld notes and Config changes.

[ptc-4940046]

Greetings,

I have been asked to create drawings useing Dual Dimensioning. I actually have two questions here. First of all, when creating weld notes, what is the industry standard for Dual Dimensioning. I have english on my primary dual in the config, and mm for my secondary. Can I add the mm in brackets on the weld notes? and How would I do that in Creo?

Secondly, How do I set up the dual dimensioning to properly reflect the decimal places. At the moment, when I set the decimal places to 3 in the dimensioning pop up box, I get three decimal places on the english, but 2 on the mm. I need 3 on both, but I have to set the dimensioning each and every time I create a dimension. Is there any way I can set it up in the config to do this automatically?

All suggestions are very much welcomed,

Thanks Ever So Much,

Diane

This thread is inactive and closed by the PTC Community Management Team. If you would like to provide a reply and re-open this thread, please notify the moderator and reference the thread. You may also use "Start a topic" button to ask a new question. Please be sure to include what version of the PTC product you are using so another community member knowledgeable about your version may be able to assist.

[ptc-4940046 · Accepted solution]

Answer to part two of my question.

file, prepare, drawing properties,

click on change that is located to the right of the detail options list.

search for dual_digits_diff

set value to "0"

click on Add/Change,

and close

on the next window, click apply and close. And another close.

This will set the default for just that particular drawing but all the dimensions to be dual and the decimal places to all be the same for both english and mm.

[TomD.inPDX]

There are variables assigned to the weld symbols. I am sure these are meant to be picked off the weld features and they may accurately show as dual dimensions.

If you are overwriting these variables, you have little option. You can either add the text you want on a single line as in:

1.0 [25.4]

or you add disassociated text and type it in yourself and then relate it to the view so it at least moves with the view.

You will find that many of the weld symbols are poorly set up for dual dimensioning. Unless you have specific instruction by policy to make everything associative, you will find yourself cutting corners around weld very quickly.

[ptc-4940046]

We are determining the weld size and adding it in at the pop up box level. It is there that I was wondering if I was allowed by industry standards to add for example... 1/4 (6.35mm). Then comes the question, if I could add something to the config to create this, but I am thinking not. I know Solid works has a welding function, but does pro/e? Never had a need for one until now.

ohhh.. should I use () or []?

[TomD.inPDX]

1.0 [25.4] or 1.0 [25,4].

If you are on Creo, you have a weld application. It takes a bit of learning but it is there. If you do this on a regular basis, you may want to make use of the provided tools. Otherwise, just know it is there for future reference.

I did test adding a dimension to a weld symbol. It works as expected... it delivers a dual dimension when you use &D0 for instance. It also works as expected as it clutters up the symbol and is basically useless.

I also made a parameter with a realnumber value and when I used this in the dialog, it did not return a dual dimension. I added &WELD[.2] where I defined WELD to be 1.0000 and it returned 1.00.

So the idea is that you can use true dimensions in the weld symbols. Cross you fingers it will present "respectably".

[ptc-4940046]

Thank you ever so much.

[TomD.inPDX]

Anytime