Convert Entities to another part

Hello;

     It seems to me that I've always been able to transfer feature edges from one parts feature to another in working in assemblies.

For some reason, I can't seem to do this right now. In other words when I'm in the sketch of the one parts feature, the edges of the

other part's feature won't highlight. Is there a setting for this, or am I missing something, or what?

Thks,

Rob_D  SW 2012

SolidworksParts And Features
Answers 20
JF
JF 2012-02-23 Best Answer

first guess - has your "dynamic highlighting" setting been turned off? (system options -> Display/Selection)

RD
RD 2012-02-23

Hello;

    Thanks for the reply. No, I can highlight, & select the edges of the part that I'm editing. Also when I'm not in the sketch editing , I can select the edges of both parts. The problem is I can't select edges of the other part when I'm editing the 1st part so I can't convert entities.

Thanks

Rob_D

PM
PM 2012-02-23

Does the other part have any constraints to any other assemblies?

RD
RD 2012-02-23

Hello;

    Yes, I overlayed the one part into the other in an assy. I mated the 3 planes of the one part I desire features from to the first part which is fixed.

Thks,

Rob_D

PM
PM 2012-02-23

Are you able to post your assembly?

RD
RD 2012-02-23

Well, they're product at a new company I'm working on, so I probably shouldn't post it. Any Ideas of what might be going on.

I seem to remember always being able to access the other geometry of other parts in an assembly, obviously.

Thks,

Rob_D

SF
SF 2012-02-23

I have learned to use "Isolate" a lot lately to do that kind of relating. Also Ctrl and Alt and RMB clicking gets me there. Be sure your options are set to allow selecting thru other surfaces.

SM
SM 2012-02-23

Robert,

What happens if you hit the "Select Other" command?

do the edges highlight then?  I have seen this happen.

If you can't post your part, can you post some images?

PM
PM 2012-02-23

When you click edit the part in the assembly, do you get a message that looks like the pic attached??

comment imagecomment image
SF
SF 2012-02-23

Do you have No External References turned on?  This will prevent that selection.  That setting is under External References/Assemblies, or if you have the icon on a CommandManager tab.

  WT

RD
RD 2012-02-23

Hello All;

     Here's some images of the situation. I am trying to simply convert entities of the green part triangular feature with the hole in it to the gray part. So I'd convert entities to make the sketch. Also scrolling down I believe shows that I don't have "no external references on".

Thks again; Rob_D

    Thanks for the input.

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AW
AW 2012-02-23

If you haven't already....  I would shut down SolidWorks and restart your computer.  It just may be stuck on that message.

Cheers,

Anna

RD
RD 2012-02-23

No; that doesn't come up

RD
RD 2012-02-23

It doesn't really give me the option to select other.

SM
SM 2012-02-23

Can you post some images of what your screen looks like in the operation?

Maybe of this component treed out in the component tree and one of the part in the

screen area.

RD
RD 2012-02-24

I don't have access to the files now.  Something that I was wondering was if this had anything to do with these being different configurations, of the same part, yet saved with different names, as completely separate files. I mean the

fact that somethings going on with the configurations. You wouldn't think so, but maybe somehow it's causing a

glich. 

SM
SM 2012-02-24

That is possible I guess.  Although when certain configs are ingaged they are not visibly present.  Which means they are not

free to select.  Maybe the thing to do is try a little experiment.  Try creating a simple assembly with just a couple of these

parts that have the configs and see if this is repeatable.

RD
RD 2012-02-29

Hello;

    I got the solution of SW, if anyone runs into this. To select the edges, you need to go to options, sytem options, display selection, then UNCHECK, enable selection through transparency.

Thks to all contributers

Rob_D

SF
SF 2015-02-16

Hi Robert,

I've just had the same problem and used your solution, so thanks for the tip.

I've just started with Solidworks and am amazed by the amount of bugs/problems with it, I wish they'd sort these out before coming up with new versions full of pointless gimmicks. I previously used solid edge, and it's a bit more basic but at least it's pretty robust.

RC
RC 2025-07-10

I learned a very useful piece of info from this 13 year old post. Was driving me crazy. Thank you Robert Dattilo if you're still alive. Just have to remember to recheck that when doing anything else but convert entries.