Every once and a while we will come across a model where there are sketch endpoints just floating out in space and they cannot be deleted. (They have likely come from a prior design iteration where the sketch was changed extensively leaving these points behind)
My question is simple, how can they be deleted?
Can you post a file that has this issue? I'm not saying I can figure it out, but I'd like to take a look.
Updated the initial post to include the file ... The points in question can be found under the "Base Extrude"
Beats me. None of the things Dan mentioned seem to work. I can select them by clicking directly on them, but a click + drag box doesn't seem to see them. I also found it odd that although they're obviously not fully defined, the sketch is showing to be Fully Defined. I'd say it's definitely a bug of some kind, but I'd probably just ignore them and go on with my life....or create a new sketch and delete that one.
I was curious to see if the points would show if I exited the sketch and set it to "Show", but for some reason it won't show up (and yes, I made sure sketches were set to Show in the "Visibility" drop-down).
I do not see the points shown in your initial post screen shot (plus the corners have a radius). Although I opened your model in SW2018 SP3.0 as I do not have SW2017 installed anymore at work.
Solid Air wrote:
I do not see the points shown in your initial post screen shot
Check your arc centerpoint and entity point options:
How embarrassing
However, I offer up this solution.
1) In the sketch add a sketch point.
2) Select one of the points that cannot be deleted and from the pop up menu select Replace Entity.
3) Select the sketch point you added and in the Replace Entity click the green check
4) The offending point disappears.
5) Click on your sketch point and select delete - poof and its gone.
6) Repeat for your other points.
At least this is how it worked for me in SW2018.
Nice, but I'd like to recommend a slight modification to that workflow. You can switch your steps 5 and 6. After replacing the first unwanted sketch point you can repeat the process with the others, using the same inserted sketch point.
This has happened to me before as well. Generally, for me, it is the result of a line being shortened until it becomes a point. The program doesn't know what to do with it.
Sometimes, if I filter for sketch segments and box select them, I can delete them.
Other times, leaving the sketch and coming back in resolves it.
Other times exiting the sketch and doing a full rebuild (CTRL Q) works.
Other times Closing Solidworks and reopening works.
Other times nothing works.
Hi John
I sometimes get these annoying points too - normally after a trim operation.
A technique I recall working in the past - but it didn't work the last time I tried - was to merge them with other points in the sketch.
I have done this in the past (merging the point to essentially make them disappear) but we occasionally work with what we call "Pin Fin" parts and there can be hundreds if not thousands of these points through the iterations which makes merging them an issue.
John Pesaturo wrote:
I have done this in the past (merging the point to essentially make them disappear) but we occasionally work with what we call "Pin Fin" parts and there can be hundreds if not thousands of these points through the iterations which makes merging them an issue.
I posted my reply below before I saw this one.
The strange thing is, you can't window select the rouge points which would make merging them with existing points a lot easier!
Interesting. Merging seems to work, except that it will always leave one point if you delete the entity you merged with. I created a line and merged the stray points one at a time with the end point of the line. When I deleted the line, one stray point was left behind.
One reason I've probably never seen this is that I don't display entity endpoints. When I sketch a line it looks like this:
So, it's possible these points exist in my models, I've just never seen them.
Rob Edwards wrote:
Hi John
I sometimes get these annoying points too - normally after a trim operation.
A technique I recall working in the past - but it didn't work the last time I tried - was to merge them with other points in the sketch.
Yup, this method works, but they don't merge with themselves.
Can you upload this file? I've never run into this behavior and I've been using SW for 20+ years.
John Pesaturo wrote:
Every once and a while we will come across a model where there are sketch endpoints just floating out in space and they cannot be deleted. (They have likely come from a prior design iteration where the sketch was changed extensively leaving these points behind)
My question is simple, how can they be deleted?
I was able to use Rob Edwards method of merging them with other points. I used the endpoints of the rectangle construction lines.
Of course this doesn't actually get rid of them but you know "Out of sight, out of mind!"
After looking at your file, you will definitely want to look at:
Crusty Old Template File Gotcha
Your part template is nearly 20 years old. Probably not related to the endpoints thing, but worth looking at.
I don't have an answer for you but I'm following this post because that has driven me nuts in the past! I hope somebody does have an answer!