How to "fix together" in a sketch?

[solid7]

I've gotten so used to the way that I do business - I need a tip for a new method...

I am doing the dxf/dwg to embossed text method. When I put the letters in a sketch, they come in at a very inconvenient location, so I need to jockey the orientation a bit.

Is there a way (other than constraining numerically) to fix all the components relative to one another, so that they can be easily moved? I want to move the text without anything changing except for the location within the sketch.

It's too much of a hassle to move externally, as reference planes tend to tie the sketch to a family, and then moving with the compass moves things you never wanted moved. (external to the sketch) It's easier just to handle it in the sketch.

Thanks in advance.


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[agumba]

u must use fiz together command. or ?n menu Insert/Constrain/constraint creation then u are going to find fix together command that u want is it enough explaining ? have a nice work..

 

[catiajim]

Rather than dragging your sketch with the compass, make it a Positioned Sketch and change the support.

 

[solid7]

Yes, I always do this - but for some reason, it still manages to catch hold of something. (even when I have isolated planes) I mean, if you change support, the idea is still to use the compass to position in in the 2 axes that are not the projection axis, is it not? (which I prefer to do inside the sketch - but I use "positioned" to flip the text)

I don't know if it's a bug, or if I just don't understand the "family" logic.

On the other hand, I can't believe that I didn't see that function. I'm ashamed. Thanks for the help.


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[catiajim]

I'm not sure. I rarely use the compass to position things in any other workbench except Assy Design, and then it's only to get the parts roughly where I need them. When working with a Positioned Sketch, I'll use a point to locate the sketch axis - even if I have to creat a point by indicating. Then, if I need to adjust it, I'll just tweak the coordinates.

Why your stuff seems to "catch hold of something", I'm not sure. You might try checking for implicit constraints. Many times I end up just turning these off, as they are almost impossible to get rid of if CATIA accidentally creates one that I don't want.

 

[solid7]

I just wanted to say that "fix together" works perfectly. Probably as you said, it has something to do with implicit constraints - but when fixing together, there is no need for any other constraint.


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[Azrael]

Have you tried to use join on the sketch in 3D and then translate?

 

[solid7]

Yes, but I like the sketch, because it's a good text "manager". That is, all the curves are self contained, and I can label the whole thing by it's text identity. Join curves force you to do one character at a time.

By the way, as a side note - has anybody noticed how much lighter the models are when you use the original polylines, extract points, and remake the letters with splines, or a series of splines? You can fillet SOOO much easier, without all of the sliver faces caused by polyline faceting.


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[strim]

catiajim
Do you ever use the snap command (looks like joined 2 spheres)
To adjust component locations. This will move component locations instantly w/o constraint. Snap together planar faces, planes, vetex, point, axis, cs and combinations of many. Quick and easy. M8

 

[catiajim]

We use snap (and multi-snap) more than anything else. I use the compass to get the parts in the general vicinity of the target, then use snap. We use snap because it works much better in a multi-level assembly (we're in VPM and it does not support Flexible Sub-assemblies).

 

[DBezaire]

I use what catiajim suggested. A point, line (for orientation) with datum on and a positioned sketch. You could use this on an isolated plane to eliminate some history.

 

[Azrael]

Solid7

If you uncheck "check connexity" the join will join element that don't meet