the slowest command in NX5 : HOLE !!!!!!!

[JBIM]

Hi everyone.

Does anyone know how to turn hole feature faster.
(Keeping the new hole command of course)

thanks

 

[hudson888]

Give us a hint here, are you on NX-5, and do you mean the new hole or the old one? What is slow about it and some background as to when and why it is a problem for you?

Regards

Hudson

 

[acciardi]

I think he means that it takes some time (10-15 seconds) for the dialogue to appear when you select the new Hole functionality. I've noticed this too.

It seems to be loading a large chunk of code into memory.

 

[JBIM]

Sorry , I submit a post earlier and forgot to mension info on this one.

I´m running NX5.0.4.1 and the problem is exactly the 15 second I have to wait for the dialogue to appear.

any sugestion ?

 

[JohnRBaker]

That issue is being addressed and so far as I and others have tested NX 6, it does appear to respond better.

John R. Baker, P.E.
Product 'Evangelist'
NX Design
Siemens PLM Software Inc.
Cypress, CA

http://www.siemens.com/plm

http://www.plmworld.org/museum/

 

[hudson888]

Yes it is a bit slow to start and there are waiting periods as it jumps back and forth in and out of sketcher. I'm not finding that it takes anything like 15 seconds but it is noticeable and could be better.

The biggest drag that I find with it is that it tends to default to sketcher too readily, but which I mean that you have to keep forcing it to use the points method if that is what you want to do. It seems if you pick a vector it will allow you to pick points, but if you thought points normal to a face seemed like a logical combination the moment you pick the face your thrown into sketcher and have to back out, (cursing at the screen all the while). Can't it remember what I did last time and not open sketcher unless I hit a specific button rather than via some intuitive behavior, that misreads my intentions.

Best Regards

Hudson

 

[JohnRBaker]

Hudson,

The biggest drag that I find with it is that it tends to default to sketcher too readily...

The sketch behavior in Holes is exactly that same as it is when using the imbedded sketcher in functions like Extrude and Revolve.

John R. Baker, P.E.
Product 'Evangelist'
NX Design
Siemens PLM Software Inc.
Cypress, CA

http://www.siemens.com/plm

http://www.plmworld.org/museum/

 

[hudson888]

John,

Yes I know but I seem to be tripping into the sketcher when I don't wish to more readily using the hole feature than the others. The reason I think is that based on previous experience the first instinct in extrude is to pick curves or sketches separately created, whereas for a hole you always picked a face first. I'm not sure what to do or set that would stop this from bugging me. At the moment I always click on vector before I do anything else the problem is that it isn't a sticky setting and it is counter intuitive as it lives on the second line and your natural tendency is to start on the top line and work down. It seems that if you click on the points icon rather than the sketch and then select a face then you somehow infer by picking the face that you want to start the sketcher. maybe I'm just mot getting something.

If I thought that it was the case that if you select the points icon and then pick some points then click on a face that it would work then maybe I would just adjust to that workflow. At the moment I'm doing something wrong and I wish that there was a sticky setting or a more deliberate click required for those of us who don't want to get thrown into the sketcher in any of these dialogs at every conceivable opportunity. Not that I terribly mind using the sketcher just that I hate having to back out or take such care to avoid it when I really wanted to do something else.

Please let me know the extent to which I'm doing the wrong thing and can change its behavior. I'm not sure whether I can set things to better suit me at this stage or whether it is just force of habit on my part.

So far I'm non-committal about the whole embedded sketcher concept and wonder whether we aren't just as well off with the two being separate features anyway. Not technically mind you just in terms of how the dialogs work seems to be trying to pack too much into one command so you're faced with two possible intuitive intents of which you have to prioritize one at the expense of the other. At the moment if there were a switch to turn off embedded sketcher behavior then I would flick it.

Best Regards

Hudson

 

[JohnRBaker]

Hudson,

At the moment if there were a switch to turn off embedded sketcher behavior then I would flick it.

For heaven's sake, don't tell an old Ideas user that ;-)

John R. Baker, P.E.
Product 'Evangelist'
NX Design
Siemens PLM Software Inc.
Cypress, CA

http://www.siemens.com/plm

http://www.plmworld.org/museum/

 

[hudson888]

Yeah they probably already hate me on here anyway!

I don't mean I don't want to have it there just to save myself from hitting the wrong buttons all the time. I may be a bit old school but I'm not so dumb I hope as to expect that I too don't have to change. I did read it back and it seemed like I wanted to do it in two steps but I didn't mean that it has to be implemented as totally separate just discrete in terms of what is assumed by the intuitive elements of the dialogs. For some reason I'm struggling with it as if it is offering the reverse of what I expect to select.

Best Regards

Hudson

 

[phillpd]

Hudson,

I'd have to agree with you that the embedded Sketches will take some getting used to and that it should be an option that the user can control. What's wrong with creating a "feature group" if you want to clean up the part navigator?

I may be doing something wrong, or not understanding the workflow correctly, but ... I was looking at your comment on defining a vector for the hole direction. I defined a vector and then selected a face (which was not perpendicular to the vector) to create and constrain my point. When I exited the sketcher, the hold preview all looked good, both direction and location. When I clicked ok though, the hold was created using the normal of the face I created.

Did I do something wrong, or am I misunderstanding something ?

Specialty Engineered Automation (SEA)

http://www.sea4ug.com

a UGS Foundation Partner

 

[hudson888]

John, and Phillip,

Thanks Phillip for your response, see I'm working my way through this better for having given it some thought. And John, I started to be conscious of what I was doing when working with NX-5 yesterday. I think that if you want to use points and not the sketcher then once I got the hang of picking the points before the face my efficiency started to improve dramatically. I think I may have been unfair in my level of discontentment. I would still prefer to require a more deliberate entry into the sketcher.

Here's a thing. The exception to wanting to be deliberate about entering the sketcher would be when editing the parameters of an already sketch based feature, obviously. I noticed that earlier I was editing the dimension parameter values during editing hole parameters, but without actually opening the sketcher. More recently however this was not available to me. Am I imagining this or perhaps did it get turned off for either license reasons or a difference between 5.0.2.2 and 5.0.3.2???

Best Regards

Hudson

 

[JohnRBaker]

Hudson,

No, the Hole sketch dimensions are available for editing when I edit the Hole without having to open the sketch, at least it works that way in NX 5.0.4.1.

As an alternative, you can also go to the Part Navigator, open the 'Details' panel at the bottom and just select (don't double-click, just highlight) the hole and all of the parameters associated with that feature (in this case the Hole) will be displayed in the 'Details' panel and if you double-click on any one of those dimensions, you will then be able to edit their value without having to even enter in the Edit Feature mode.

John R. Baker, P.E.
Product 'Evangelist'
NX Design
Siemens PLM Software Inc.
Cypress, CA

http://www.siemens.com/plm

http://www.plmworld.org/museum/

 

[hudson888]

John,

Just to confirm both worked perfectly as I had seen earlier. I don't know what it is with the other machine that I was using. It appears that I won't be able to go back and test it out for a couple of days. This was one of the Dell boxes that the IT guy was saying had problems which he may or may not have "fixed".

Anyway as it stands the intended functionality is good in the respect that it is quite easy to use etc...

Best Regards

Hudson

 

[NXMold]

I'd like to turn off the "default into sketcher" behaviour myself. I rarely sketch within the extrude or hole dialog, and often cancel out of sketches due to my sloppy selection skills. The current default is an impediment given my workflow, I would prefer to hit the sketch button when its needed. I thought that the setting in customer defaults, modeling, general, misc tab would do this, but it dosent seem to. Is there another option somewhere to tailor this to my style of working?

I think that requiring a more deliberate action to enter sketcher is justified by the time it takes for sketcher to open, and to back out.

Or is there a way to de-emphasize face selection?

 

[hudson888]

The thing is that half of this office are still on NX-3 and it may be some time before we move onto NX-5 and after that even longer before the next upgrade. By that time I gather from my experience that like a few dialogs that threw us to begin with we'll have got used to using whatever we're stuck with. I'm already finding that while it isn't perfect I am starting to get the hang of the hole dialog.

Regards

Hudson

 

[idaho100]

COPY/ PASTE of hole features is much speedier than hole dialogue. …..assuming a multi-hole layout? ill-suited for arrays? (AND I don’t know anything about nx5/6; but NX4 hole dialogue was also too slow: SO this may be considered an “ NX 4 method”
1) do complete hole layout with a SINGLE sketch, just define all target positions as POINTS for that face or orientation ( constrain sketch points now or later) ;
2) Apply hole function once to any sketch POINT ,
3) Copy/ Paste that hole feature to remaining points. Helps to us APPLY button, user repeatedly hits APPLY button , this way dialogue ‘stays put’ , ready for next PASTE,
This is much faster .. for Initial definition , much faster for positional editing etc.
Side point --- helps to have hot keys defined for UG APPLY button , this is something everyone should have anyway … use keyboard button(s) to APPLY, forget mouse clicking any dialogue box, is huge time saver.
Maybe new NX5 / 6 hole stuff faster, I don’t know, but I somehow doubt it.

 

[hudson888]

Stan,

What key to you map to Apply?

Regards

Hudson

 

[JohnRBaker]

A benefit that perhaps you're not aware of is that IF you first create a sketch containing multiple points, constrained or otherwise, and you then use that sketch when you create your holes (you select the sketch using the 'Feature Points' selection intent), if you go back and add or remove any holes to the original sketch, the number of holes update automatically. Granted, the sketch of points will not be 'managed' automatically (hidden until the holes are edited) nor will any constraint dimensions be editable from within the holes dialog, but it does separate the two tasks, defining the hole locations and defining the holes themselves, which might provide a more efficient work-flow.

For example, if I knew I had to create a large number of holes on the face of some part, I could first create a sketch with perhaps ONLY a single point, then create your hole by selecting the 'Feature Points' even though it's only a single point. Now you can continue to work on your model and when you're ready to finish up, just go back and edit the original sketch adding the additional points and constraining them and when you update the sketch all of the additional holes will be created.

One other thing to note is the when you create your sketch you can include any number of extra lines or arcs to help constrain the locations of the points and they will be ignored by the Hole function, even if the curves are NOT first converted to reference objects.

John R. Baker, P.E.
Product 'Evangelist'
NX Design
Siemens PLM Software Inc.
Cypress, CA

http://www.siemens.com/plm

http://www.plmworld.org/museum/