metric to imperial on a IDW
Hi
Go to the description tab, select all dimensions and change their style to imperial in the list.
Kacper Suchomski
YouTube - Inventor tutorials | LinkedIn | Instagram
Did you find this post helpful? Feel free to Like this post.
Did your question get successfully answered? Then click on the ACCEPT SOLUTION button.
Hi @robert_barnes22. Do you have any existing dimension styles that are already set to imperial units? If not, then it may be a good idea to create at least one, just for occasions like this. This is because the 'Units' of our drawing dimensions are actually set within the dimension style settings. If this is not familiar to you, then while you have your drawing open, click on Inventor's 'Manage' tab to activate it, then click on the 'Styles Editor' tool, which is within the 'Styles & Standards' ribbon panel. That shows a large dialog with style categories on the left, and settings related to the selected items on the right. If you expand the 'Dimension' category, you will see at least one dimension style there. One of those is the currently 'active' one, which gets applied to all 'new' drawing dimensions that you create. If you do not already have an existing dimension style that is set to imperial units, then you can create a copy of one of the existing dimension styles, then change its units to imperial units, and change any other properties you may want to. Then click the save button at the top of the dialog, then the save and close button at the bottom right corner. Now, in the 'quick access' toolbar (usually in Inventor's title bar) there is usually a tool button with a little drop-down arrow next to it (like in the screen captured image below). Click the drop-down arrow, then slide down and click on the 'Select All Inventor Dimensions' option. Doing so selects all drawing dimensions on the active sheet. Next, click on Inventor's 'Annotate' ribbon tab, and if you have the ' Format' tool showing in your ribbon, you can just use the bottom drop-down list (list of available styles) to switch the dimension style of all selected dimensions to the new one you click on with imperial units. Doing so should change all of those dimensions so they are showing imperial units. Below are a couple screen captured images from my screen, but I have an American/English installation of Inventor, so most of my dimension styles are already using imperial units. You usually do not want to edit the 'active' dimension style for something like this, because doing so will affect all of the new dimensions you create using that dimension style, and may actually not change the ones that have already been created using that style.
Wesley Crihfield
(Not an Autodesk Employee)
Hi! There is an easier workflow to do the conversion. Before attempting it, make a backup copy of the drawings.
1) Open the target drawing.
2) Go to Manage -> Standards and Styles -> activate the Imperial standard (ANSI). Now there should be two local standards.
3) Go to the tree view on the left and find Object Defaults -> expand it -> right-click on the Metric Object Defaults -> Replace Styles -> pick the Imperial Object Defaults.
All the style-driven annotations will be changed to the new standard.
Many thanks!
