I want to get to a detailed view of a part on my drawing, but it is an internal region of the part. This means I have to do a section view, and then a detailed view of the section view to get to the view I want. I tried the Auxiliary View option, but this seems to only do external views of parts (even if the View direction indicator arrow falls within the part – see the drawing).
Is there a way to get an internal view of the part?
I have put my current efforts on a simple mock-up part to illustrate the issue as clearly as possible (drawing and part attached).
Solved! Go to Solution.
I know, not exactly what you're looking for, BUT, have you considered using PMI Sections? Removes the need for extra views in the draft layout.
When you have a view placed, it behaives like assembly configurations, but there is a separate tab in the view properties for "Section"...once a PMI Section is created, it is listed, and chech the box next to the one you want.
Thanks SeanCreswell for your solution. That helped. In the end, I took a while to get the hang of PMI Section view, so it wasn't the easiest solution (blame my ignorance).
With the help of EDGE plm software's excellent support (http://www.edgeplm.com.au/support.html) of which I am a customer, the best solution for me was the one shown in the attached video. A basic description is:
a) The desired area we want a magnified view of is hidden inside the part. Right-click on the view, and on the General tab, click the settings to make hidden lines be drawn as "visible".
b) Adjust the outline box as necessary to obtain an image of the detail area only
c) If the scale of the desired area is too small, right-click on the drawing view, and click "Delete Alignment". Now the Scale dropdown box will be adjustable in the PromptBar.
No problem...glad a solution that works for you was found.
As a supplement to that work flow by EdgePLM, try clicking on "Maintain Alignment" [just toggles that alignment off/on, and no other clicks needed, and better still, alignment can be restored by repeating that process] instead of delete. Plus, if there happened to be unwanted visible geometry that passes through the resized model view frame, sometimes I use the "Hide Edges" tool, on the home tab, to remove as desired.
Actually, that alignment part and scaling (in the video) was my own clumsy technique, not EDGE plm software's suggestion. They just helped me give the "hidden" dashed edges a "visible" edge style. Your right-click on the drawing view > deselect "Maintain Alignment" tool is much cleaner. Thanks for taking the effort to watch the video and improve my Solid Edge techniques.
I use the "Hide Edges" tool often. On the "hide edges" topic, is there a way to automatically hide all "hidden" (dashed) lines in a drawing view, rather than hiding them manually?
...is there a way to automatically hide all "hidden" (dashed) lines in a drawing view, rather than hiding them manually?
I guess, not showing hidden detail in the view[s] at all, would do this easiest.
Either set up in the draft template to be like that for all new drafts, or just on a per view requirement.....via the view Properties, on the "Display" tab.
Thanks Mark for your excellent video (including helpful audio). I have only just started using broken out views, and your video demonstrated how to make them very quickly.
It is yet another way to get my desired ending. All I need to do at the end of your video is cut out and scale up the area I want to detail (without having a full section view). I've realised I could have made my mockup a closer in size to my actual part, which would probably have explained to all the helpful Solid Edge experts why I needed this specific area detailed as I asked.
Thanks everyone very much for your time and effort. I now have my drawing looking exactly as desired, communicating clearly with the manufacturer, and my supervisor gave it the thumbs up yesterday. It was an issue we didn't know whether Solid Edge could handle, but it turns out the software is more than capable.
P.S. By the way, I am very impressed with Solid Edge's video feature. It makes sharing ideas far easier and quicker than typing out a guide with pictures! The audio on your video makes things even easier to understand. I'll have to find a microphone somewhere!
I now have my drawing looking exactly as desired, communicating clearly with the manufacturer, and my supervisor gave it the thumbs up yesterday.
Excellent!....and THAT my friend, is what it is all about, right?. "Getting the job done!"