Tek-Tips is the largest IT community on the Internet today!
Members share and learn making Tek-Tips Forums the best source of peer-reviewed technical information on the Internet!
-
Congratulations TugboatEng on being selected by the Eng-Tips community for having the most helpful posts in the forums last week. Way to Go!
NX 5 Hole feature launches sketcher ???
- Thread starter tburcha
- Start date
JohnRBaker
Mechanical
The new Hole feature is designed to be used WITH the Sketcher as the primary means of defining parametric locations of holes, unless you already have locations defined using some other means. This could include selecting existing points or some other object, like a curve, where you can use Snap Points to define a hole's location. But if you have NOTHING that you can currently use to define a hole's location, exactly how was it that you were expecting to define it?
Now that being said, since you have at your disposal ALL of the Snap Point options, you could have toggled ON the 'Point on Face' method, which will, to some extent, emmulate the pre-NX 5.0 behavior, EXCEPT that you will NOT be given the chance to define location dimensions, as that's what we intend that you use the Sketcher for.
And note that this is not a unique behavior nor even new behavior in NX. For example, when creating an Extrude or Revolve feature, if you have NO predefined profile or set of curve/edges suitable to be used in an Extrude/Revolve operation, you are automatically taken into the Sketcher where you can define a profile or network of curves suitable for Extruding/Revolving. This same approach is used throughout NX Sheet Metal and is being found in other workflows as well such as when creating Variational Sweeps and an Emboss feature.
This approach of defaulting to creating a Sketch when there was nothing appropriate to select, either as profiles or locations, is going to continue to be the norm for NX and will eventually be incorporated, where applicable, in other NX functions as they are updated and brought up to the new workflow and dialog standards.
John R. Baker, P.E.
Product 'Evangelist'
Product Design Solutions
Siemens PLM Software Inc.
Industry Sector
Cypress, CA
To an Engineer, the glass is twice as big as it needs to be.
Now that being said, since you have at your disposal ALL of the Snap Point options, you could have toggled ON the 'Point on Face' method, which will, to some extent, emmulate the pre-NX 5.0 behavior, EXCEPT that you will NOT be given the chance to define location dimensions, as that's what we intend that you use the Sketcher for.
And note that this is not a unique behavior nor even new behavior in NX. For example, when creating an Extrude or Revolve feature, if you have NO predefined profile or set of curve/edges suitable to be used in an Extrude/Revolve operation, you are automatically taken into the Sketcher where you can define a profile or network of curves suitable for Extruding/Revolving. This same approach is used throughout NX Sheet Metal and is being found in other workflows as well such as when creating Variational Sweeps and an Emboss feature.
This approach of defaulting to creating a Sketch when there was nothing appropriate to select, either as profiles or locations, is going to continue to be the norm for NX and will eventually be incorporated, where applicable, in other NX functions as they are updated and brought up to the new workflow and dialog standards.
John R. Baker, P.E.
Product 'Evangelist'
Product Design Solutions
Siemens PLM Software Inc.
Industry Sector
Cypress, CA
To an Engineer, the glass is twice as big as it needs to be.
- Thread starter
- #3
JohnRBaker
Mechanical
Trust me, we did NOT have to do this to JUSTIFY the Sketcher. Please show me any other system out there that depends on its 'sketcher' less than NX does. And while it may be true that the Sketcher is becoming the preferred way of defining parametric profiles and locations, in most all the cases where this is the default, we still offer ways to select profiles and locations which do not depend on the Sketcher (again, show me any other system which does the same).
John R. Baker, P.E.
Product 'Evangelist'
Product Design Solutions
Siemens PLM Software Inc.
Industry Sector
Cypress, CA
To an Engineer, the glass is twice as big as it needs to be.
John R. Baker, P.E.
Product 'Evangelist'
Product Design Solutions
Siemens PLM Software Inc.
Industry Sector
Cypress, CA
To an Engineer, the glass is twice as big as it needs to be.
- Thread starter
- #6
Why did only the Hole feature change and not slot, boss, groove or pocket?
I put four holes located on each corner of a block with a horizontal and vertical dimensions of zero. The blocks lower left corner is a 0,0,0. Then I try to relocate them. Upper right and upper left holes relocate without an issue. Lower right and lower left no dice. It won't move these because the sketcher won't accept negative values and a positive value moves it off the block. Also, it takes more clicks to locate the holes. Just don't see the improvement. Maybe still better than other systems but ...
I put four holes located on each corner of a block with a horizontal and vertical dimensions of zero. The blocks lower left corner is a 0,0,0. Then I try to relocate them. Upper right and upper left holes relocate without an issue. Lower right and lower left no dice. It won't move these because the sketcher won't accept negative values and a positive value moves it off the block. Also, it takes more clicks to locate the holes. Just don't see the improvement. Maybe still better than other systems but ...
- Thread starter
- #7
JohnRBaker
Mechanical
We have not yet initiated a project to update the Slots, Grooves, Bosses, Pads, etc., features to the new style dialog, but when we do it's safe to assume that they will get a similar treatment as you have seen with the NX 5.0 new Hole feature project.
As for you sketch dimension issue and not being able to edit the 'zero' values in such a manner that you get your desired result, from the NX 8.0 'What's New' document:
Sketch dimension enhancement
What is it?
Perpendicular, Horizontal, and Vertical driving Sketch dimensions now maintain their direction when the expression value is set to zero. You can also enter negative values for these three driving dimension types to achieve the same results as using the Alternate Solution command.
John R. Baker, P.E.
Product 'Evangelist'
Product Design Solutions
Siemens PLM Software Inc.
Industry Sector
Cypress, CA
To an Engineer, the glass is twice as big as it needs to be.
As for you sketch dimension issue and not being able to edit the 'zero' values in such a manner that you get your desired result, from the NX 8.0 'What's New' document:
Sketch dimension enhancement
What is it?
Perpendicular, Horizontal, and Vertical driving Sketch dimensions now maintain their direction when the expression value is set to zero. You can also enter negative values for these three driving dimension types to achieve the same results as using the Alternate Solution command.
John R. Baker, P.E.
Product 'Evangelist'
Product Design Solutions
Siemens PLM Software Inc.
Industry Sector
Cypress, CA
To an Engineer, the glass is twice as big as it needs to be.
Singsonite
Automotive
Maybe I haven't given it enough of a chance yet, but I have had to find ways to work around the sketcher up to this point. Doing things like creating associative datums and intersection curves to produce parametric, selectable intersection points on surface. I know that wasn't the intent, but it's quick, easily definable, and easily adjustable. I try hard not to use the Pre-NX5 Hole command, but sometimes it makes more sense to me.
My company works with some very large files. When I wanted to update the location of a hole or series of holes in the past, it was as simple as changing the dimension of a datum plane. Having to edit a sketch from inside a large assembly to change my hole locations wreaks havoc on our systems.
I don't know....maybe I'm doing something wrong. I will have to go back and revisit the newer hole command until I am more familiar with it.
John B. Conger
Tool Design
Automotive Interiors
Advanced Engineering Solutions Inc.
My company works with some very large files. When I wanted to update the location of a hole or series of holes in the past, it was as simple as changing the dimension of a datum plane. Having to edit a sketch from inside a large assembly to change my hole locations wreaks havoc on our systems.
I don't know....maybe I'm doing something wrong. I will have to go back and revisit the newer hole command until I am more familiar with it.
John B. Conger
Tool Design
Automotive Interiors
Advanced Engineering Solutions Inc.
JohnRBaker
Mechanical
Starting with NX 7.5 you no longer have to actually open a sketch to edit the dimensions in the sketch (this pertains to not only Hole features but also Extrude, Revolve, etc.).
So in the case of a series of holes created using a sketch, when you edit the holes, whether you use the simple 'Edit Parameters' option or you use 'Edit with Rollback', when the Hole dialog is activated you will see all of the dimensions used in the sketch to locate the holes even though you are not actually in the sketch task. At this point you can simply select any of these displayed dimensions, edit the value and the location of the hole will update. The only time that you will need to enter the sketch task itself is if you wish to add or remove holes, or you need to edit the original scheme used to define the location of the holes.
In fact there's even a general purpose option in NX 7.5 where you can temporarily 'turn on' the sketch dimensions used to create a feature without having to even enter the feature edit dialog. And while these dimensions are displayed they can be edited and the model will update.
And we can go even one better by making the sketch dimensions into PMI dimensions (which in NX 8.0 can be done right from inside the sketcher as you're adding them), and since PMI objects can be ON all the time, if I'm in modeling I can simply double-click a PMI dimension and if it's a driving dimension (which sketch dimensions are by definition) I'll be able to edit its value right there without having to first open any sort of dialog or launch an explicit edit operation.
John R. Baker, P.E.
Product 'Evangelist'
Product Design Solutions
Siemens PLM Software Inc.
Industry Sector
Cypress, CA
To an Engineer, the glass is twice as big as it needs to be.
So in the case of a series of holes created using a sketch, when you edit the holes, whether you use the simple 'Edit Parameters' option or you use 'Edit with Rollback', when the Hole dialog is activated you will see all of the dimensions used in the sketch to locate the holes even though you are not actually in the sketch task. At this point you can simply select any of these displayed dimensions, edit the value and the location of the hole will update. The only time that you will need to enter the sketch task itself is if you wish to add or remove holes, or you need to edit the original scheme used to define the location of the holes.
In fact there's even a general purpose option in NX 7.5 where you can temporarily 'turn on' the sketch dimensions used to create a feature without having to even enter the feature edit dialog. And while these dimensions are displayed they can be edited and the model will update.
And we can go even one better by making the sketch dimensions into PMI dimensions (which in NX 8.0 can be done right from inside the sketcher as you're adding them), and since PMI objects can be ON all the time, if I'm in modeling I can simply double-click a PMI dimension and if it's a driving dimension (which sketch dimensions are by definition) I'll be able to edit its value right there without having to first open any sort of dialog or launch an explicit edit operation.
John R. Baker, P.E.
Product 'Evangelist'
Product Design Solutions
Siemens PLM Software Inc.
Industry Sector
Cypress, CA
To an Engineer, the glass is twice as big as it needs to be.
Singsonite
Automotive
Excellent! It at least sounds like we are all on the same page and working toward a similar goal. I can't wait to sample the improvements for myself.
Thanks for the feedback.
John B. Conger
Tool Design
Automotive Interiors
Advanced Engineering Solutions Inc.
Thanks for the feedback.
John B. Conger
Tool Design
Automotive Interiors
Advanced Engineering Solutions Inc.
- Status