Does anybody have any experience in using and controlling cross-hatching in WF3? In previous verision of Pro-E We'd use datum curves or cosmetic sketches and select X-hatch. We could then control the appearance of the X-hatch either in the part or in the drawing. In WF3, you can create a cosmetic sketch and select a X-hatch, but then you have no control over the parameters of the hatch (number of lines, spacing, angle, etc.) We use these features in creating mechanical reference features like ECAD keepouts, surface finish areas,etc. This is a very frustrating omission in WF3, and we may be faced with having to go back to our previous version of Pro-E. 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.
Hi paul, you can control the appearance in drafting. just double click on the cosmetic - xsection you have created, you will get the options to change the appearance like spacing, angle etc... Rgds SPP
One of the other users was trying to crosshatch an assembly, and there seems to be a glitch. you can't change the crosshatch pattern, angle or spacing of the individual parts seperately. I tried to help him figure something out, to no avail. Anyone else experience this?
Here are my notes for how to create/manage cross-hatching in WF3. 1) Create a sketch on a surface as you normally would do. 2) Once completed, Edit Definition of the sketch - Once in Edit mode, Select "Sketch" and then "Sketch Setup..." from the pull down menus. - Under "Sketch Setup..." Use the properties tab to select X-Hatch and adjust the Spacing as needed 3)In Drawing Mode you can edit the properties of the sketch feature to adjust angle, spacing, etc. but you must have the config setting "draw_models_read_only" set to "no" for this to work. - Set the config line "draw_models_read_only" to "no" - Select and right click the hatched sketch and select properties from the pop-up menu. This will bring up the traditional hatch control dialog menu