How do you snap onto objects

[engibeer]

Im used to solid works solid edge and autodesk inventor. Im starting to try out catia v5. How do you snap lines onto objects when drawing new objects in sketch mode or when trying to move a sketched object? I cant seem to do this.

Say you already have an extruded part. Then on a surface you do another sketch that will be used for extrusion or cut. How do you snap newly drawn sketch objects to the extruded geometry?

 

[TibiX]

Hi engibeer,

This [link youtube.com/watch?v=zRgAw_zxgkI] simple tutorial[/url] will probably help you more than any of my written words...

P.S.: This guy has a lot of simple CATIA tutorials and are gold for a beginner.

Best of luck!


CATIA V5R21 – mold tool design engineer

 

[engibeer]

THanks for the links. I just looked at the video and it doesnt seem he did any snapping onto previously draw objects. It seems he was using the grid snapping and he drew objects using multiples of the grid size so it worked out, but if it was some fractional value he wouldnt have been able to snap with the methods he used.

I think I figured out a way that seems to be as close as what I am used to with other CAD. I used the "project 3d elements" command to project existing features first, then I was able to use those lines for some feature snapping. I dont know if this is the normal or preferred or only way of doing this. In other CAD you they normalyl allow snapping of the same part objects right away.

 

[TibiX]

You can just use an edge or a face when giving a distance. If that doesn't work for you, your CATIA settings are at fault.

Projecting isn't wrong but consumes time when you shouldn't.

CATIA V5R21 – mold tool design engineer

 

[engibeer]

What do you mean by giving a distance? Do you mean using the 'constraint defined' commands, where you already have an object drawed and you want to define relationships relative to other lines?

Do you mean you can snap onto features when doing that?

What I mean is not have to go through the extra annoying step of doing the constraint method, but being able to directly draw the geometry (e.g. circle or rectangle or line) directly on the object and have it be able to snap onto the existing object and relationships (e.g. center of an extruded circle or center of a line feature etc).

Now, I can snap onto features provided it is still the same sketch. It doersnt work if the object has already been extruded from a previous sketch.

The only way I seem to be able to do this is to project the element first.

 

[TibiX]

There is no "snap" when you draw in a sketch. But when you apply the constrains there is no need to project existing elements.

CATIA V5R21 – mold tool design engineer

 

[DaSalo]

CATIA seems to be set up around a pretty linear workflow where you sketch all of your geometry first and then dimension and apply constraints second. It is not as efficient to mix the two as it is in some other systems. Once all of your geometry is on the screen you can just double click the dimensional constraint icon to keep it active and apply all of your dimensional and geometric constraints at once without ever leaving the command. To apply a geometric constraint you just right click to reveal the menu with the context appropriate constraints. As has been previously mentioned, you do not need to project geometry into the sketch first. You do need to get comfortable with the idea that your geometry will be sitting unconstrained for a longer period of time than it would in other systems because the more efficient workflow tends to front load all of the sketching and backload all of the constraints. It took me a bit to get used to this but I think it is probably just as fast once you get comfortable with it.

CATIA V5 R20
PC-DMIS 2011 MR1

 

[engibeer]

I know you can ultimately create the same geometry after dimensioning and constraining drawn features. But this is ridiculously slow. In other programs that allows snapping, you can simply draw construction lines etc and rely on these to quickly and efficiently create drawings.

Im still convinced catia must have this ability but I cant seem to find a setting to unlock it to be able to do this. Or does it not and the only way to snap onto existing features is with the "project 3d" command?

 

[DaSalo]

It really does not have it. At least not that I am aware of. Sketching in CATIA requires a very different workflow than sketching in Solidworks or NX.

CATIA V5 R20
PC-DMIS 2011 MR1

 

[jadieki]

In your sketch you will have to intersect or project the 3d edge or feature. If the lines created are yellow they will be linked to the surface you intersected. So if the surface moves the lines in the sketch will go with it.
personnaly I wouldn't create the sketches on an existing surface, I would create a plane from a datum plane in the same place and then create the sketch on that. depending how complex your parts are, if you start creating sketches on existing surfaces it will cause frustrating problems later on.
I haven't used solid works though so hope that helps.

 

[Albigger]

Also be careful when using the "project elements" or "intersect elements" while in sketcher. While this will allow you to "snap" to an existing feature, sometimes this causes a lot of headaches later on. For example, if you project a surface, then later on come back and change that surface (with a fillet, for example), CATIA will sometimes (often) "lose" those projected elements. I find the more "update-friendly" approach is to do this, for instance: If you have an extruded cylinder, made from a sketch of a circle, and now you want to sketch something else that also has the same size circle, I go back to the original sketch, un-hide it, and constrain my new sketch to that old sketch (concentric and coincident). I would not constrain to the surface of the extruded cylinder, and would not use the project 3D elements button. Again, this is highly dependent on your modeling practices and what you will be doing, but we get a lot of very complex models that need to be updated several times, and this helps keep the tree from blowing up with errors during updates.

 

[DaSalo]

Albigger gives good advice here. My general rule is to never create an associative link (sketch projection would be included in this category) with anything that is not visible in the tree. If it doesn't have a name that you can see and modify then you can be pretty sure that CATIA will break the link at it's first available opportunity.

CATIA V5 R20
PC-DMIS 2011 MR1