question regarding sketch contraint, projection

[godpaul]

Hi all,

After one day self-learning of NX, i got some sketches problems

1,the first one is why NX tells me i need to have additional two constraints even though i know that two those constraints NX needs are 2 reference lines. In some cad software, reference line, aka construction lines are not dimensioned, or not necessary. dont know why NX needs this requirements

2. is there a better to project line or curve? what i did is just hit the project curve button in the sketch environment, and you can see picture. however, this has shortcoming as even though i try to project lines, they will be treated as "spline".... I found this issue because i think those projected lines will be lines and when i try to make other hand-drawn line parallel with the projected "lines", nothing happens....

3. why there is no extrusion cut, sweep cut, revolve cut, in all, everything related to "cut" is not found in NX...
i have to create geometries and then do subtraction. Is NX designed in this way? what's the benefit?

4. whenever i create a sketch, a window popups, asking me to define plane and coordinate. If, for some reason, after I finish teh sketch and realize that i draw sketch on the wrong plane, i want to redefine the plane but do not want to re-draw everything, how to proceed? I tried to right click on the sketch in the Par Navigator like i did in other cad software but didnt have similar options...


thank you for all your support. Learning NX is a little challenging but will keeping going

picture for constraint

http://files.engineering.com/getfil...13269e364426&file=constraint_of_reference.PNG

pic for projection of a curve

http://files.engineering.com/getfil...9c-b579-48cfc8e23739&file=project_a_curve.PNG

 

[jerry1423]

1. NX does not REQUIRE really anything in a sketch, you can do what you want with a sketch even if it's under=-dimensioned or under-constrained
2. it really depends on the application
3. no you don't have to create it, and then subtract (in a separate feature), if you expand your menu fully you will more than likely see the options that you need to do what you need in one operation.
4. There is a way to do this, but I am not at my work computer now. But look up "reattach sketch"

As a newbie I need to point out to you the Command Finder. It is very handy and you can even enter the command on your previous CAD system and it will do its best to find the NX equivalent.

Don't forget to specify what version of NX you are on.

 

[godpaul]

Hi jerry1423

I am using NX 8.5

couild you elaborate more about your reply to Question 2

if you want to project a line, or a curve from another external sketch, what did you do usually?

thank you

 

[godpaul]

for your reply 1, i forgot to mention,
yes, i can do whatever i want in sketch but I always bear in mind that a good practice is to make sketch FULLY CONSTRAINTED, not under/over constrained.

since it's firt time that i encountered NX which suggests reference lines to be dimensioned according to the sketch top window message. So i dont know if it is OK to leave reference lines un-dimensioned.

 

[godpaul]

sorry, i need to be careful,
if a reference line is inclined, it must have to be dimensioned with an anggular dimension...

 

[JohnRBaker]

The issue with respect to 'reference curves' (they can be more than just lines) is that once you leave the Sketch and use it to create some sort of topological feature, that the 'reference curves' will NOT be considered as part of the sketch profile. This means that while you're right that it will still be good practice to fully constrain them along with the rest of the sketch curves, they do not need to be created to some specific SIZE, particularly in the case of LINES.

For example if you've created some reference line to represent say the centerline of some shape, there may not be any needed to actually add a dimension for it's length since the length of the line it irrelevant. I mean whether the line was 10 mm or 1000 mm long, it would be just as effective for use as a centerline with other curves/constraints/dimensions using it for reference (hence the use of the term 'reference curve'). If you don't want to add an actual length dimension that will clutter up the sketch try using a 'Constant Length' constraint. This will fix the length of the line without the need for an actual dimension constraint. And if say one end of the line is already located where you want it to be there is no need to add dimensions defining where that end point is located, just select and apply a 'Fixed' constraint and again, as the name implies, that end point will be locked down (i.e. constrained) to that location. And if you have the line both where it needs to be and the length/angle is OK, you can lock down EVERTHING by using a single 'Fully Fixed' constraint which will lock down the location of the end points, the length, the angle, everything, without adding a single dimension to clutter up or confuse the diaplay of the sketch.

Anyway, look carefully as some of the non-dimensional constraints available to you as they are often useful particularly when working with reference curves that do not have to be constrained to a specific SIZE or LOCATION. They can help immensely when it comes to help fully constrain your sketch while reducing the clutter of adding additional dimensions which adds no value to the sketch itself.

John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Industry Sector
Cypress, CA
Siemens PLM:
UG/NX Museum:

To an Engineer, the glass is twice as big as it needs to be.