Hello, Im currently trying to fix a problem I'm having with a few parts made in wildfire 3. The problem is that I created models for a client using their startpart/template, and I thought that this would take care of any differences between their configuration settings and mine, but it didn't:) The problem is now that when I send the models to the client the dimensions in the modelling window doesn't display as they want. So I got their configuration settings, both config.pro and config.sup to try and fix the old models that I created so they display as they should. I have replaced my config.pro files with theirs and when I create new parts everything looks as the client want but when I open one of the old models they don't display as they should, even though the options window show that the clients config.pro is loaded. So I'm assuming that the old models have some kind of information in it's file that overrides the new config settings so what I'm hoping is that their is someone who can help me to figure out how to apply the new settings to the old files without having to redraw them. Would appreciate any suggestions anyone can give me. Thanks Tobias 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.
Hello, are you talking about a 3D model or a drawing? For a drawing you could have to load a new drawing options file (File>Properties>Drawing Options>Open) I'm using WF3, so I'm not sure I'm able to help you
Thanks for the reply Sylvain, Its the dimensions that you can turn on in the modelling window, by right-clicking a feature and then choose edit. The config.pro settings I got from the client made it possible to display the dimensions in the modelling window as nominal even though the display tolerances is checked under Tools>enviroment. They had their reasons for why they wanted it this way. This works fine when I create new parts but when I open an old part with the new settings loaded it still displays the dimensions the wrong way(as limits instead of nominal). Me and some co-workers fixed the problem today, by changing all the dimensions in all the models manually to nominal. But I am still interested if there is anyone who know if there is some way you can force old files to use "new" configuration settings.
As far as I can tell no they can't be forced to use the new Config.pro settings. There's a note in the help that states that groups brought in from other models have the tolerance display mode that was in effect when they were created. So I think the only way to change them is the way you are currently changing them.
Tobias, There are basically two configuration options that are driving the dimensional display. They are : tol_mode :- limits,plusminus.... tol_display:- yes or no. For models that had the features made in one mode & if you want to convert them to other you can select all the dimensions & change the tolerance for all. To do that: #Edit >> Find >> Look for -> Dimension & Look By -> Dimension.Then hit 'Find Now'. Then select any one dimension in the window & press CTRL + A to select all the dimensions. Then pick the arrow key in the center to select all.Close the window. Then hit the right mouse button in the graphics area & you will get the properties tab,press it and here you can change the limits for all dimensions & the tolerance mode too. Please be aware that this will modify all the dimensions with same tolerance limits & class. You can make a mapkey to perfrom the same operation in different models.. Rameet