Thanks again for taking the time to read and possibly answer my questions.
How can we acquire the ASME standard for Creo 3.0, and maybe 4.0 versions? Currently, we have ANSI and ISO standards, but we use ASME for most assembly and part GD&T. What's the best way to get ahold of a license, standard file for ASME in Creo?
Second, we also use a lot of the fit tolerances (h7, H7 pin/hole size), but it isn't available for ANSI for our installation. Is that a separate file as well?
Last question, we also started noticing assembly files that we get from customers, their parts seem to have different units. We usually operate in Millimeters, but noticed some parts may have been set to inches or sometimes Centimeters. Is there a setting to set all parts/assembly files in the structure to one unit?
Hopefully this wasn't too much to ask, but thanks again reading. I'll be looking forward to any responses.
There are several places online you can buy ASME standards, including ASME website...The American Society of Mechanical Engineers
Y14.5 is the dimensioning and tolerancing book. Y14.100 is top level one that lists all the other related standards.
(The standard used to be ANSI and has since been renamed to ASME)
I'm not a fit tolerance guy so I can't answer that one.
You can convert the units once you bring them in but you would do them basically one at a time, there is no conversion setting.
file - prepare - model properties - units - change
First Question: You are going to have to be more specific. Creo supports ANSI, ISO and ASME but there are no files for them. For instance if you look at the drawing detail option gtol_datums the options are std_asme, std_ansi and std_iso among others.
Second question: If you are referring to hole sizes, those can be controlled with the .hol files. You can create those on your own. More info here:
Thanks Chris and Stephen for your quick replies.
With our Creo installation, we only have ANSI and ISO (std_iso, and std_asme), and that is all that is shown in Options list. Sorry for not being specific, but I'm looking for std_asme for Creo 3.
I think I found a request in another forum that basically tells me my answer. As far as using a Fit Tolerance, it's not yet supported for ASME standard, only ISO and DIN.
There are multiple options in drawing setup for ASME/ISO/DIN/JIS for various purposes.
Are you just specifically looking for fit tolerance options? I don't understand exactly what you are asking.
I'm sorry, the one question I have right now is to get the ASME standard in Creo 3.0. I'll have to wait to see if I can create the Fit Tolerances when I get that std_asme file.
1. I want to create GD&T or Annotations in the 3D part/assembly. However, the only standards I have available are ANSI and ISO standards. There are no ASME standard or std_asme files available.
Otherwise, reading some past forum posts, fit tolerances cannot be created in the with the ASME standard, here is the link: Tolerance table support for the ANSI/ASME tolerancing standard
Did you look at the gtol_datums drawing option as I suggested? You should see the std_ASME option for that. What option is it that you are referring to that does not have a std_ASME that you are looking for? Not all options are controlled by ASME which is why there isn't an option for it.
Its a drawing detail option (like a config.pro only for drawings). From the drawing in the search bar search for "detail options" without the quotes.
You're not missing anything. ASME is fully support (with a few minor exceptions). Look at the option Chris suggested. Also, there are several other options. Look under file-prepare-model properties-detail options change from within the part or assembly.
OK, so I created a new assembly, went to Prepare - Model Properties and was able to find and change the Standard.
I did also check where Chris suggested. In the Drawing Options and the Detail Options. I found the gtol_datums and could just enter std_asme. So, doing so will change that in drawings, or would it change throughout Creo's Config file?
I might be chasing ghosts here, but after this post I do realize Creo allows users to create GD&T pretty much how they want them. The Standard setting doesn't block, change, or set a default to the Datum Reference Frame or apply the Envelope Rule.
Changing that value in the drawing options only effects that drawing. It does nothing to other drawings that are already saved. If you want to save this for drawings going forward, you can set the config.pro option drawing_setup_file to a file location (ie c:\dwg-setup.dtl) so that it will effect all new drawings going forward. If you want to retroactively apply this change to saved drawings you can open a saved dtl file from the drawing options dialog box. Note that all settings from the file you open will override any existing drawing settings if do this.
Most of what you do to use a standard is to set your detail setup file to use <loadpoint>/text/iso.dtl, /jis.dtl, /prodetail.dtl for ASME, and to have your start/template files using the standard you like. The standard templates assume ASME for inch models and ISO for mm models, but you can set it up as you like.