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Sketches in an Assembly

Hi Everyone,

I'm new here, and quite new to Solidworks. Just trying to find my way around. It is a little different to my usual software and I get a little frustrated sometimes when I know what I want to do, but can't quite work out how Soldiworks wants me to do it. Going quite well, but I've hit a bit of a brick wall, that I hope some of you old hands can help me through.

I have constructed an assembly from various parts, so far so good. But I want to trim an outer case to the outline of some batteries contained within it. Dead simple trim, just requires a circle to be cut out of a pad standing up on the case. I can easiy create a sketch on the end of the battery, but cannot use it to trim the case. When I try to use the sketch to trim the case it tells me the sketch must be linked to the part I'm working on, and the sketch is linked to the battery, not the case. How should I be approacjing this?

Thanks for any help,

Kevin

Reply to
Kevin Steele
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Highlight the "case", then pick "edit part", then make your sketch on the "battery" face and trim the case.

Mike Eckstein

Reply to
Michael Eckstein

But when I selected "edit part" all the other parts in the assembly (critically, the battery) became transparent and I couldn't select anything on them, it only seemed to let me work on the part selected. Have I got an option set wrongly for doing this (I haven't got the hang of all the options -there seem to be so many of them).

Regards

Kevin

PS

Just had a thought, could I draw the circle >Highlight the "case", then pick "edit part", then make your sketch on the

Reply to
Kevin Steele

Go to TOOLS OPTIONS and under SYSTEM OPTIONS choose the DISPLAY/SELECTION option. Then under the ASSEMBLY TRANSPARENCY FOR IN CONTEXT EDIT choose the MAINTAIN ASSEMBLY TRANSPARENCY. This will remove the transparent parts that your not editing.

Reply to
Jo

Sounds like you have the option "No external references" selected. That would prevent you from creating the type of reference that you want. For me, that button is on the command manager toolbar, but is probably also accesible (insert spelling coorection here ) through the menus. If I recall correctly, it is on by default.

If that was not the case, selecting transparent items can be tricky. Try hovering your mouse over the area where your battery face should be. Right click and chose "select other", hovering over the selections in the box that opened up should highlight the appropriate face, then select it. Sometimes rotating the view to a different orientation ( one in which there are fewer possible selectable items under your cursor ) can make the selection easier.

Reply to
Brian

re: Selecting entities in an assembly while with other parts transparent

Go to Systems Options > Display/Selection > check "Enable selection through transparency" box You will now be able to select the desired edges of transparent parts

Or With "Enable selection through transparency" not checked. Hold down your shift key and move the mouse pointer over the desired edge, it will highlight. The shift key reverses the role it plays in selecting entities.

Kman

Reply to
Kman

Kman, You have that backwards.

Kevin, You need to what Jo has suggested. I fought with this for a long time until I figured it out. Actually I think someone figured it out for me as well.

Muggs

Reply to
Muggs

Thats it -thanks. By holding down the shift key it lets me select edges/faces from the other parts while sketching in the case part. I thought it would be simple -but finding it isn't!.

Regards

Kevin

Reply to
Kevin Steele

The part about "enable selection" is backwards as you noted. Thanks for pointing that out.

Kman

Reply to
Kman

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