Cancel
Showing results for 
Search instead for 
Did you mean: 

Holemaking

Pioneer
Pioneer

This is really two questions..

 

How does one tag points or surfaces to be recognized by NX as a user specified feature such as a tapped hole etc. I tried playing with it but everything comes up as a 1/4-20 hole or similar and I don't see many options to change them. 

 

Is this feature documented somewhere in detail? .. besides just mentioning that the possibility exists? 

 

Anyone using this feature? 

 

 

15 REPLIES

Re: Holemaking

Genius
Genius
Hi turuleng,

There are two geometry types to distinguish:


A: Points and Arcs
There is point tagging and arc tagging. The issue with these older commands is they add attributes to the tagged object when you select the point or arc. At selection time you have to choose any of the primitive features (SIMPLE_HOLE, etc.) and the values chosen specify the attibute values set on the geometry. When the point or arc moves (e.g. with a part), then the attributes remain the same. This can lead to a hole machining tool path that is at the wrong location or uses the wrong tool axis.
A better solution is to use a HOLE_BOSS_GEOM parent in which you select the point or the arc.
In both cases you will get new tagged features in the MFN, but you can change the parameters (diameter/depth) of the object from within the HOLE_BOSS_GEOM. In NX10.0.1 it seems to me there is an issue with geometry that has been moved, because there are cases when the tool axis is not changing, but only the starting point of the hole.

B: Cylindrical Faces
Even if you just have a cylindrical face, but want to machine a thread/tap, you should use this kind of geometry. In the tapping or thread milling operation, you can choose thread from model, set a user defined thread depth and machine a thread on any cylindrical face. Depending on the topology, NX recognizes STEPx or similar features. If the topology does not match a feature type, the cylindrical (or conical) face gets recognized as a tagged feature. When the tagged geometry moves, everything moves along properly.

It takes some time to find the best way. You have not stated which NX release you use. Depending on the version things may be quite different.


Best regards,
Joachim
Best wishes,
Joachim

In production NX 11.0.2 MP1 D1
In testing NX 12

Re: Holemaking

Pioneer
Pioneer

I could never make this work. It is a very cumbersome. It is a neglected  feature but it could have potential. I assume this does not work with NPT tapped holes.

 

I am using 10.0.2.6.

 

 

Re: Holemaking


turuleng wrote:

I could never make this work. It is a very cumbersome. It is a neglected  feature but it could have potential. I assume this does not work with NPT tapped holes.

 

 


Several solutions were suggested - which one are you referring to here?

Which ones have you tried?

Mark Rief
Retired Siemens

Re: Holemaking

Genius
Genius

Hi turuleng,

 

Can you please tell me what kind of geometry you have in your example part?

 

Solid body without any holes?

Solid body with holes but no symoblic threads/taps attached to it, but you want to machine the thread/tap?

 

Let´s clarify this and then take the next step. It really depends on what you want to achieve.

 

Best wishes,

Joachim

Best wishes,
Joachim

In production NX 11.0.2 MP1 D1
In testing NX 12

Hole Machining on Datum Points

Genius
Genius
Hello again,

please let me share all information I have about hole machining on Points.

Location definition:
Let me propose to always use HOLE_BOSS_GEOM objects to tag the point location. In most cases you have several operations to machine a hole (spot drilling, drilling, countersinking, tapping...). I think you can ignore the default diameter and depth values. Maybe it would be beneficial for hole milling or thread milling to specify diameter and depth.

Hole machining:
Set the machining parameters in the Feature Geometry sub dialog. Use MODEL_DEPTH with Position by Shoulder. This, by default, sets the shoulder of the tool to the point. So you would just machine with the tip. Use a negative Bottom Offset to set the depth to machine by shoulder. With this approach the depth is independent from the position.

Tool Axis:
This is the not so perfect part. The tool axis is taken from the hierarchically (is this a real word?) lowest Main MCS. This fact probably kills using Points at my site due to postprocessor restrictions.
You can change the feature orientation manually. Do this in the HOLE_BOSS_GEOM object. In the list of features (cylindrical entities with a tip called NXHole) you select the one you want to give a different orientation. Then click on the orientation button. The axis system of the feature is shown in 3D. Use the handles to change the orientation. Although the axis system doesn't look like it supports it, you can select e.g. the Z-axis and then a linear or planar geometry. This immediately aligns the axis with the geometry. From what I was able to figure out you have to do this for every feature position you want to reorient.

Today, there was not sufficient time to perform more tests with hole machining milling operations.

I hope this helps machining on points. The guys at Siemens are doing a really good job.

I did my tests on NX10.0.1.4 with some extras of NX10.0.2 .
Best wishes,
Joachim

In production NX 11.0.2 MP1 D1
In testing NX 12

Re: Holemaking

Genius
Genius

Hello turuleng,

 

I don´t know what the "NPT" in your reference to tapped holes means, but let me share the following information about machining tapped holes:

 

If there is no NX symbolic thread attached to a cylinder you still can machine it with hole machining operations.

 

Choose the cylinder you want to machine the tap on.

Tapping: You choose the right tool. In the Feature Geometry dialog leave Form and Pitch = From Model. The only thing you have to specify is the parameter Thread Length because it can´t be determined from the geometry. All the other thread related information is taken from the tool.

Thread Milling: Choose the tool you want. In the Feature Geometry dialog leave Form and Pitch = From Table. Then you don´t need to figure out parameters Major Diameter and Minor Diameter of the thread. Specify the parameter Thread Length as for Tapping.

 

This should be it. If you would have thread information on the cylinder of the hole, then NX would tell you if thread pitch of your tool does not match to the one of the modeled thread.

 

The whole thing also works on Points, Arcs, non-STEP-feature cylinder (if any) taken with e.g. a HOLE_BOSS_GEOM. Depending how you did it you need to specify diameter and depth.

Best wishes,
Joachim

In production NX 11.0.2 MP1 D1
In testing NX 12

Re: Holemaking

Esteemed Contributor
Esteemed Contributor

NPT = National Pipe Thread

NPTs are tapered threads.

 

Not sure if his hole geometry is modelled as cylinder or conical face.

but in any case, if you are thread milliing, go to the section where you choose the thread std, and see if NPT is there.

 

Ken Akerboom Sr CAx Systems Engr, Moog, Inc.
Production: NX10.0.3.5 MP5 + patch/TC11.2
I'd rather be e-steemed than e-diseaseled


Re: Holemaking

Pioneer
Pioneer

Joachim

 

This is lots of good info and thanks for taking the time to put these down. I have been travelling so I have not had a chance to try these but I will. 

 

My beef with all this that this is not a well documented feature.

 

I think what you are describing, and correct me if I am wrong, that the user has the option to  gather all the similar arcs or faces together though some filtering ( diam / radius )  and tag them with the thread parameters?? 

 

This would be great...How one is supposed to figure this out from the manuals and looking at the UI is beyond me though.  My initial guess was that this was supposed to be a one by one tagging which is hardly productive. 

 

The majority of the files I work with comes from Pro/e as step files, I am not sure what to do with your "when holes move comment". People in the contract manufacturing business usually work with static files that are not connected to the design cycle. 

 

I will try these suggestions though. 

 

Thanks

 

Re: Holemaking

Genius
Genius

Hi turuleng,

 

do the parts you need to machine have no holes or no threads/ taps defined?

Best wishes,
Joachim

In production NX 11.0.2 MP1 D1
In testing NX 12

Learn online





Solution Information