Adding Holes In NX7.5... 2

[4mranch6]

Alright, a technique I used to use in NX4 to locate hole features was to creat a sketch on or off the plane the hole would reside on. With this sketch displayed (Layer on.) I would open the hole feature dialog menu and specify the desired hole dimensions. Then select the face the hole was to be located on and then select a point on the sketch as the location point. Hole would be created in the solid as desired. Editing was simple by just adjusting the original sketch as desired.

In NX7.5 I have yet to figure out how to replicate this process. It seems as though the sketch must reside on the face on which I want the hole to be loacted.

Can anyone please give me some advice on how to do this?

Thanks.

 

[4mranch6]

Here is a workaround I used for now, but it just seems to add an extra step that was previously not required. I used my sketch to extrude a small hole (OD smaller that the ID of my desired end product hole.) thru the solid and then I could use the center point of those hole features to locate my end product hole, which in this case was a counterbore hole.

 

[JohnRBaker]

OK, you've got a couple of choices. The first one is to NOT use the 'Normal to Face' Direction option, but instead use the 'Vector' option. Of course, in this case the 'depth' of the hole will be measured from the actual point that you selected, but if you're creating Through Holes that's not going to be an issue.

The second approach would be to go ahead and select the face that you wish to place the holes, as if you were going to create sketch points on the face, but instead of defining new points, just select your existing off-surface points and they will automatically be projected onto the selected face and will be used to define the origin of the holes. And they will be associative so editing any of those original off-surface points will cause the actual points being used by the hole function to update as you would expect them to.

John R. Baker, P.E.
Product 'Evangelist'
Product Design Solutions
Siemens PLM Software Inc.
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[4mranch6]

Your second option is the route I was attempting to take, but I always ended up with 2 holes. The first being at the random point where I selected the face and then the second at the projected point location that was where I really wanted the hole.

Your first option works with thru holes, but would not work with holes to a depth, counterbore, or countersunk holes that required starting on a particular face.

 

[JohnRBaker]

In the second option, which is very close to what happened prior to NX 5.0, all you need to do is DELETE the point which is automatically created when you first select the face of your model.

As for the first, yes it's only practical for through holes, but if you're creating non-through holes or one which require a starting face, then use the second option as that's virtually the same as how pre-NX 5.0 worked, except for having account for that extra point which is only a couple of extra actions, select the point and hit the 'Delete' key.

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

http://www.siemens.com/plm

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

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

 

[4mranch6]

Option 2 works as suggested, thanks John.

 

[DaSalo]

That first point that gets created when selecting the placement face really is a bit of a pain. I would guess that I delete it in favor of some other placement scheme nearly 95% of the time. I design tooling, and that generally means lots of screw and dowel holes, so that 95% really adds up. What is the logic behind that first point being automatically created? It is hard for me to imagine many situations where that would really be much of an advantage and it is a very palpable disadvantage for what I do. Are there any customer defaults that can eliminate that behavior?

 

[JohnRBaker]

What version of NX are you running? With NX 7.5, that first point, as well as any others created, will be automatically dimensioned meaning that it will be fairly easy to edit it's location without having to perform any additional operations.

As for why we implemented it this way, originally the first point was not actually being created until the user had confirmed the entry, but so many people ended up thinking that a point had been created that they would enter the point creation step and then leave it before the point was accepted forcing them to start over. Finally, after testing this with users, both internal and actual customers, it was decided that it would be better to ACTUALLY create that first point as part of the face selection action. Besides, with the advent of the 'auto-dim' behavior in NX 7.5, the consensus was that even if the point was in the wrong place, it would now be fairly easy to edit the location, so the fact that a point was ALWAYS created was now seen as only a minor issue.

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

http://www.siemens.com/plm

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

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

 

[FrankMalone]

If you don't want the firs point, when enter in the hole dialog, select the sketch section icon, select the face and OK now you can select the points for the holes.

Regards
Frank.

 

[capnhook]

I think it was a bad decision to create the first point as part of the face selection step. Anytime you end up with two holes, when you are expecting one, is more work and more than a minor annoyance.

It has got to be driving tool designers batty to have to delete that "free" hole all the time.

If, during testing, a few users were being confused as to whether a point they created was being accepted, I'm sure that after banging their heads against the wall a couple of times, they could learn the correct way to use the hole creation tool.

Instead, the development team makes a decision to hamstring ALL users with the unwanted hole feature.

Dumb.

Proud Member of the Reality-Based Community..

 

[DaSalo]

I'll check out the behavior in 7.5 I've been using 6.0 predominately but could upgrade if there is a compelling reason.

Frank, that is what I do most of the time. However, I like the idea of being able to just click my placement face and have the sketch environment open. I just don't want any sketch tools to launch automatically. More often than not I'm placing 2 or more holes at once and I do it by drawing lines and using the endpoints, drawing rectangles and using the corners, etc. I don't often place just one point so even with auto dimension I would delete that point and draw a rectangle instead most of the time. If I am placing a single point it is usually because I want a counterbore coming in from a face that is opposite some already existing hole. In that case I usually do an associative point projection instead of placing a point and then constraining it coincident.

The automatic behavior must be great for someone's purposes or it wouldn't be in there. I just wish I could turn it off or change the tool that automatically launches if I want to.

 

[JohnRBaker]

Unless you're running NX 7.5 you are NOT seeing how it's intended to work. After all, if you're creating holes and you enter the Sketcher, exactly what was it that you were expecting that you were going to be doing there anyway? Aren't you going to be creating points for the holes? So what's the big deal about the first point already having been created? As I said, in NX 7.5 it will already be dimensioned so that all you need to do is edit the sketch dims to define the desire location.

And if you really DON'T want to create a point (but then why are you even in the Sketcher) you can follow the workflow described by FrankMalone, but it will require an extra button push. As an alternative, if you do happen to select the face with the intention to sketch some points but you don't want the point which was created automatically, just press MB2 and then Ctrl-Z and it'll be removed and you can then continue to sketch whatever you wish.

Which brings me to this; you say that this was a "bad decision", however if we update and modernize some legacy function, but it requires an extra button push or selection, we get criticized for adding extra steps. In this case we designed the function so as to save button pushes and what happens, no one notices that but rather they are surprised by the fact that one action, selecting a face, resulted in something unexpected, a point being created (one that you'd eventually have to create anyway). Well that's the sort of thing you have to do in order to save button pushes. If we already know what the most likely NEXT ACTION is going to be, in this case, creating a point, why would we NOT go ahead and perform that operation automatically

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

http://www.siemens.com/plm

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

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

 

[JohnRBaker]

BTW, just because that initial point has been auto-dimensioned does not mean that you couldn't immediately create a line/rectangle and then using the Constraint command, 'move' that first point to coincide with a line endpoint or one of the corners of the rectangle. If you do that, the auto-dims on the point are automatically discarded.

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

http://www.siemens.com/plm

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

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

 

[capnhook]

Saving button pushes? You made more of them....did you count the ones you need to press to get rid of the (always) unwanted hole??

You're darn right --- the result is ALWAYS not as I expect.

I'm learning to expect that.

Proud Member of the Reality-Based Community..

 

[DaSalo]

For the record, I actually don't think it is a bad thing at all that there is an automated behavior such as this. I just wish I could have some control over exactly how it behaves. In some projects I might want automatic single point creation. In others I might want the default to be something else. My only comment is that if an automatic behavior is provided it would be helpful for me if I could make some adjustments or turn it off.

 

[capnhook]

I agree, DaSalo.....and remember to put me in the "turn it off" category, then.

Proud Member of the Reality-Based Community..

 

[kimrivers]

What I am failing to understand is where the WCS for the sketch is going to end up being. I pick a face to insert a simple hole and it seems if the sketch wcs ends up in a different location than I expect. I would like to locate holes not from any edge of the face or another existing hole but the datum 0,0,0, of the casting , pre machined..How can I do that from the beginning rather than trying to tweek the location that the system has seemingly arbitarily chose? Thanks..just started on 7.5 and I am the only full time modeler at this location so no one else to ask.

 

[kimrivers]

Right now I am just letting it put the hole wherever it decides..then go to drafting, dimension the hole to find where it is in relation to my datum points , then go back to modeling and tweek it till it is where I want it. Very tedious way to create a hole..

 

[mmauldin]

Once you pick a face, the sketcher automatically (and seemingly arbitrarily) selects a horizontal reference and origin point. However, while in the sketcher you can select Tools>Reattach which gives you the option to select whatever horizontal reference and origin point you desire.

You will also see the alignment reference triad. Double clicking any of the direction arrows will reverse the direction of that axis

 

[JohnRBaker]

While it may at first appear to be 'arbitrary', when using the 'Inferred' method for defining the plane and orientation of the Sketch, the system attempts to find some logical place to create the origin, such as a Vertex Point for a face with straight edges, Center Point for a circular face, etc. As mentioned, if you use the Sketch origin tools you can assign it however you like. Note that once you get the feel for how the 'Inferred' option works, you will find that you can usually get exactly what you want while saving several keystrokes.

John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Industry Sector
Cypress, CA

http://www.siemens.com/plm

UG/NX Museum:

http://www.plmworld.org/p/cm/ld/fid=209

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