Best practices for sketch & models in NX

[201181]

Hi,

I'm quite new to this forum, but even in the short term I've been using it, I have found it incredibly useful.

I am currently using NX, and am working in a company in Denmark as a contractor. I have been using NX for approx 1 year so far, with many years experience in other systems from Catia to Creo pro direct.

I was just curious about the best practices that should be employed when creating sketches and models. I have a procedure I follow for creating my parts, and I was curious if this was the preferred/correct method of other more experienced NX users on here. My procedure is as follows:

1. If starting a model with a sketch, I will place this on the DCS (Datum Co-ordinate System) as inferred, using the X axis as my horizontal ref. If using a primitive, I use the centre point and the X axis of the DCS as my axis.
2. When starting a sketch, I will create it away from the DCS and complete all constrains/dimensions apart from two that constrain it to the DCS (If making a round hollow part, I will add a centreline as a reference line, and constrain all my diameter dimensions to this). I then completely constrain my sketch to the DCS as a last step.
3. If making a round part, I will revolve using a line within the sketch as my axis. If making a square part, I will of course just use the DCS as my extrusion direction.
4. After this, all other features are constrained to the model I created from the sketch or primitive. If required, I will add datum planes, axis and curves to the part model to ensure I get correct placement of all new features, with no associativity to the DCS.

Is this the way that everyone else does it? Is there any disadvantages with doing it this way? I'm just very curious to see what others practices are. Another reason I ask this is because I have noticed that other users in the company I am working at do not worry so much about how they create their models (many features could be associative to the DCS for example, but for me, this does not make a very robust model).

Many thanks in advance.

 

[Toost]

In my opinion , the described is good practice.
, It can of course vary depending on what you are about to design , would i start from a point cloud or do freeform shape design it's not that definitive.
but for general machinery details , it's recommended.

Regards,
Tomas

 

[SDETERS]

. After this, all other features are constrained to the model I created from the sketch or primitive. If required, I will add datum planes, axis and curves to the part model to ensure I get correct placement of all new features, with no associativity to the DCS.

How are you putting your datum planes? Are you using surfaces of the part to define your Datum planes? We usually offset most planes and or reference features from that first Datum Coordinate system?

 

[201181]

Toost: Nice to hear that it sounds like standard practice

Sdeters: This is an area that I am not 100% sure if I'm doing it right (opinions would be most appreciated here)... I place the datum planes onto the surfaces of the revolve/extrude/primitive. If its a planer face, then I would typically use inferred (directly on the surface) or at a distance, and if on the diameter/radial surface, I would use tangent or on curve, and if going through the centre of the part, I would use through part.

I am interested in datum placement on diameter/radial surfaces alot because lately, I have been creating a lot of models where a hole has to be placed onto a radial surface. My method for placing such a hole is:

1. Place a datum using on curve or tangent on the outer diameter/radius.
2. Place another datum on the end planar face (or sometimes at a distance to the planar face).
3. Place a datum axis through the centre of the part.
4. Place the hole using the hole feature, I create a sketch point inside the hole feature dialogue/sketch on the datum described in point 1, use a dimension from the planar datum described in point 2 (or on point constraint if the datum is offset from the planar face), and add an on point constraint for the point to the datum axis described in point 3.
4. Now I have a fully associative hole position, with no reference to the original DCS.
)
I have also done all the above using datum planes to make section curves (no sketches) then use the intersection snap function when placing the hole in the hole function dialogue.

Does the above sound like overkill to anyone out there?

Thanks again!

 

[SDETERS]

My theory is anytime you use a face to define something (datum plane, coordinate system) the model becomes fragile or not robust. That is why fillets fail all the time. The fillets are associated with Edges that change number constantly in big complicated models.

Could you provide a model for an example above? Have you looked into using expressions to use to place these planes?

What is your thinking about no associativity to the origanl DCS? What Version of NX are you using?

 

[201181]

Most of the NX methods I was taught was via a colleague when I worked at another firm as a contractor (this was when I first started using NX, and the colleague had been using it for many years at large automotive companies), so this is all I know. I remember this colleague hd created a design manual for the firm we worked out, detailing a procedure for constructing models in NX, and he was very adamant that every feature after the initial revolve/extrude/primitive should be fully constrained to this initial model.

His example of why something should not be constrained to the DCS after the initial was that if the initial sketch or primitive was moved, then all other features would loose their associativity to the model. A good test was to move the primitive away from the DCS when the model was complete. If the model still updated, then the model was robust. But I would love to hear any advantages their may be with keeping features associative to the DCS. I am just trying to improve my usage of NX, and hopefully teach others.

I would love to provide a basic model, but it will have to wait until next week now as I'm home for the weekend

 

[ewh]

Tying the features to the DCS is great if you use expressions extensively, so any editing is simply a change to an expression (so say if a boss moves, the hole moves with it without having to be directly tied to the boss, or visa-versa).

“Know the rules well, so you can break them effectively.”
-Dalai Lama XIV

 

[NutAce]

1. Place a datum using on curve or tangent on the outer diameter/radius.
2. Place another datum on the end planar face (or sometimes at a distance to the planar face).
3. Place a datum axis through the centre of the part.
4. Place the hole using the hole feature, I create a sketch point inside the hole feature dialogue/sketch on the datum described in point 1, use a dimension from the planar datum described in point 2 (or on point constraint if the datum is offset from the planar face), and add an on point constraint for the point to the datum axis described in point 3.
4. Now I have a fully associative hole position, with no reference to the original DCS.
)
I have also done all the above using datum planes to make section curves (no sketches) then use the intersection snap function when placing the hole in the hole function dialogue.

Does the above sound like overkill to anyone out there?

Hi..

Don't know what version of NX you are using but this is indeed a bit overkill...
For placing a hole feature on a cylindrical plane you only need 1 Datum plane...The one you are placing your hole.
The hole features internal sketch gives you all the posibilities to fully constrain the position of your hole center associative to your models geometry or the WCS.

As you are alreay creating your main body associative to the DCS ( or ABS Csys ) I would also use this to create your diemensional constraints. Using your models geometry might give you some issues if geometry is modeled away by other features later on.


Ronald van den Broek
Mechanical Engineer
Cad Environment Coordinator
Wärtsilä, Propulsion Services
NX8.5.2 / TC9.1.2
HPZ420 Intel(R) Xeon(R) CPU E5-1620 0 @ 3.60GHz, 32 Gb Win7 64B
Nvidea Quadro4000 2048MB DDR5

 

[201181]

Hi Ronald, many thanks for your reply. yes, perhaps my modelling methods are a bit overkill, so it's nice to hear others opinions on how things should b done in NX.

Here is an example part of my taught modelling methods. Any feedback would be most appreciated from anyone reading this

 

[NutAce]

Hi..

Nothing wrong with this particular case..Using datumplanes here is a good and quick way of pistioning and it wil make sure that the hole is always in the middle of the cylinder...
One drawback though....if you ever need to change that..then it would be much easier if you had a fully constraint sketch...

I have added a hole on the oppposite with just 1 datumplane. the position of that hole is driven (in the sketch expressions ) by the length of the cylinder. (position = p1/2)
Doing it like this I can change that just by going into the expressions and give it a fixed value ( or even give it a more detailed formula ).

Change the formula for Position to;

if (p1 >= 100) (30) else (p1/2)

And change the length of the cylinder to 120.

This can be done with datum planes as well of course but you need an xtra datum plane to accomplish this.
The hole feature is already creating a sketch, so why not use it to it's full potential.




Ronald van den Broek
Mechanical Engineer
Cad Environment Coordinator
Wärtsilä, Propulsion Services
NX8.5.2 / TC9.1.2
HPZ420 Intel(R) Xeon(R) CPU E5-1620 0 @ 3.60GHz, 32 Gb Win7 64B
Nvidea Quadro4000 2048MB DDR5

 

[201181]

Hi, many thanks. I do also use sketch expressions for certain features, but one thing I do like about using datum planes for positioning of holes is that it's more obvious how the position is controlled compared to using in sketch expressions (at least for me it's more obvious, but it may not be to others as you don't need to open the sketch/expression dialogue to find the expression). But of course, like the drawback you have mentioned, it's not so easy to change if you one day didn't want the hole midway between the two end faces of the part.

Many thanks for your input

 

[SDETERS]

Here is how I would model the part. I do believe each person has their own modeling style. I always say different strokes different folks. If you also look you can move the second coordinate system and the original first feature will move with it. This was done per your comment above.

Also if you go back in and add a fillet/draft to the end of the cylinders the part will not fail.

 

[201181]

As you say, everyone has their own style to modelling (for me, it's important that the model is as simple as possible, with separate defined features in the tree to make it easy for someone to modify in the future).

I'd never though of using an offset CSYS. It is actually another good way of doing it. I'm not 100% sure though why, but I do remember a former colleague telling me to never use more than one CSYS in a part. Why would it be a problem?

As for the counterbore hole made from a sketch, I do prefer to add a datum plane onto a diametral face, then set the depth from that so I know I always have a defined depth from the diameter in, and not from the centre out (I know you could set something up with expressions. but it takes more work and is not as simple for someone else to understand, if the model needs to be modified in the future). Again, each to their own methods and it's good to see another perspective

I can see the point about adding a chamfer to the part (before the datum planes) could cause it to fail. However, I only ever add chamfers at the very end of the part tree. But it will make me think a bit more about how I position holes in the future.

Thanks again!