Hello to all - (Edge-Flange4 bottom cable support) in this part does not want to flatten. Interesting that the mirror of the same bend does. I'm fairly inexperienced in SW so any help would be appreciated.
Chris,, Somewhere, Somehow, "EdgeBend4" got suppressed. Unsupress it. I also removed the hole at the bend from Sketch9 (made it construction geometry) then added it back in after your Edge-Flange4. Must admit I was a bit surprised to see this work without errors. I'm using 2017, hope this will work in 2012.
One other item you will need to deal with is that SolidWorks does not flatten forming tools (cable form tool2). At the end of flat pattern folder you will see a Sketch Transformation1 folder which contains a sketch that SolidWorks cannot resolve. I would recommend suppressing the forming tool feature since it really is not part of the flat pattern anyway?
On a different note.....corrupt file issue
This is a good example where the SW flat pattern is corrupt. You can see that in the above image. the light grey surfaces are missing.
The merge faces options in the flat pattern feature causes this problem. I see this issue with SW sheetmetal parts more and more.
While it's no problem in the model it cause havoc in assembly drawings that remain in draft mode for ever. If you run the check function you can see the faulty faces. SW does not highlight these errors & they are real hard to track down in large assemblies. Most of the time SW will list the error in the Result list column. The arrow indicating the error will often point into empty space and no details are provided what part or component is affected. Maybe SW can work on the problem itself and the error checking report. A isolate function would be great so items with errors can easily be identified.
Food for thougth
I don't see any issues Elmar.
Edit:.. While I'm on this.. I disagree with Solid on having the form show up in the flat pattern. It is a hit just like all the holes and cut-outs and will be there when the part comes off the turret. Also it makes it convenient to dimension the form if you are planning to use the flat pattern in your drawing. I never do it myself but others do. You can change how that is going to work in doc properties. Show form tool profiles, Show form tool punches, Show form tool centers, etc.
SolidAir has the issue and I have it too. It can be seen looking at the image. When I saw SolidAir's image, I knew it had errors.
To check for errors you need to enable "stringent" option which is unchecked in your image. I'm not sure what causes it, but it seems to happen on other installations too (see SolidAir). Also I can reproduce it if I select merge faces. It doesn't show up when merge faces is unchecked.
Maybe that helps...
I do understand what you are saying Elmar. As I indicated in my first post, adding the hole (right at the bend of "Edge-flange4" after the edge flange solves the issue. When it is created prior to the edge flange there is a problem. As you can see in my screenshot I do have "merge faces" on. You are correct I did not have Stringent on during my check but it makes no difference. The trick is moving the hole after the flange.
I can see from the image below when the graphic issue occurs. The first image has errors (red arrow indicates light grey missing surface) the other not. Look at the bent tab in the bottom left corner or the holes. You can see the difference between faces that work and the ones that have graphic errors. The difference is the merge face options being active in the first one and not in the last. This is the default file as downloaded without any changes. I don't know what causes this. I know it happens most often with Sheet metals but can occur in other SW part files as well. Another contributing factor is when multiple configurations are present.
The main issue is drawings. I just recently had a file where is used a reference surface that had knitting issues. The surface is an offset surface created in context. The error points into space in fig1. That's what I get originally. In Fig 2 I have selected the hidden surface feature you can see it points to the error. So the error is not much help in fig 1. Now look at the top level assembly as seen in fig 3. How do i identify what part is the problem. You have to look for it manually because you can't really tell what part is the problem. These errors only show up when stringent is selected. The main issue is that it occurs more often then I like. And it really cost a lot of time to troubleshoot if drawings are affected. The drawing shows no sign of error. It simply remains stuck in draft mode....that's the clue.
To resolve the error I simply added a delete feature to remove the surface at the end of the feature tree and the errors are gone. The surface are simple in nature. Just a corrugated sheet with tangent bend sections and a straight extrude. Why SW can't handle the most simple type of surface offset is another questions. What is interesting that once the surfaces were removed then my drawing view resolved fine.
I simply make note of it so others have a way to trouble shoot. The forum has often pointed me in the right direction and maybe this article can help someone.
I actually did not do a full analysis of the model. I still have SW 2012 and I all I did was check if Dennis' solution would work in SW2012 since he was using SW2017 (I forgot to mention that I used SW2012 in my post because I got distracted by the sketch transformation which has only caused issues where I work).
Policy where I work is flat patterns are flat. 99% of our sheet metal models do not use forming tools so I am unaware of the show tool profiles, punches, centers, etc. (so I will need to look at that).
To Dennis and everyone else - thanks very much for the fix. As with most SW things the answer very simple once you see it.
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