-
Re: positioning an inserted part
Right click the inserted part and click "Edit Feature". At the bottom of the list of selectable items is a box called "Locate part with Move/Copy feature". Select that, and it should let you locate your part.
-
Re: positioning an inserted part
Patrick
Your approach is essentially what I do, except I don't find the option to move when I select a part,
so I have to select a face, request the move, deselect the face and select the part to do the move.
Kelvin
Good refs for the docs. However, I can't find the point to point move (vertex). All I have is the X,Y,Z,
or select an edge for directión and input a distance. That will be accurate to within a mil, but its not
exact. I can't get the vertex optión to show in the translation reference. What am I doing wrong?
Thanks to both
Guy
-
Re: positioning an inserted part
Go to insert, features, move/copy bodies. in the top box select the part to move. You can use the arrows shown on the screen and drag them. Also if you select the box at the very bottom called "constraints" this will show mate settings such as coincident, parallel, tengent ext. You may have to use the move command mor than once to move you part. Tom
-
Re: positioning an inserted part
Done, works.
So the sequence is insert/features/move-copy
then select the body and specify the mates.
Thank you. Just couldn't dig it up in there.
-
Re: positioning an inserted part
Yes that is it. You can also rotate and translate the body if needed. I am not sure what you are working on. I was using this command to remove material from the inside of a larger part where the inside was an odd shape. I found that the command "cavity" works well also. It is a little wierd to use though because you have to create an assembly and edit the part. Tom
-
Re: positioning an inserted part
Guy Pommares wrote:
So the sequence is insert/features/move-copy
then select the body and specify the mates.
If you have this box checked when inserting the part, you won't need to add the extra move body feature. It's what Patrick was talking about in his post.
-
Re: positioning an inserted part
Tom
Are you saying that with the 'cavity' command you can substract one
complex shape from another; like if you wish to make a mold for instance?
Glenn
Good point. Very helpful. Hadn't scrolled down that far.
Guy
-
Re: positioning an inserted part
Guy,
Yes, you can use Cavity in an assembly to subtract one part from another, as in making a mold. There is a similar function that you can use in a part, the Combine feature, to add, subtract or intersect bodies.
Jerry S.
-
-
-
-
Re: positioning an inserted part
Thanks for sharing this Tom!!!
That is why I love this forum...you literally learn something new every day
Chris
-
-
