cancel
Showing results for 
Search instead for 
Did you mean: 

Hole Making Questions

Valued Contributor
Valued Contributor

Is there a way to pick all holes on face by min/max diameter like when using point to point? I can't seem to find a way to do it. I know that hole making is the way they're going from now on, but I can't find a workflow that isn't really slow. I also can't find a replacement for engage/retract along tool axis with a distance. That one is very useful on our 5-axis mill. About all I can find is an automatic plane with safe clearance distance which isn't as controllable.

7 REPLIES

Re: Hole Making Questions

Valued Contributor
Valued Contributor

Find the parametric features in the machining feature navigator, then select and sort by the diameter column. When the CAM operation is open, you can highlight items in the feature navigator to select. Select the whole range of a specific DIA by holding down shift key and selecting the range2017-05-19_1625.png

Production: NX 11.0.1.11 MP2 Primarily CAM

Re: Hole Making Questions

Esteemed Contributor
Esteemed Contributor

What NX release are you using? For the future you may want to add your environment to your signature to stop other members having to ask for it Smiley Wink

The new drilling has a different work-flow than the ancient P2P:

  • for single holes you can still select the geometry directly inside of the operation
  • for multiple holes it is best to start with the machining feature navigator

The work-flow for the machining feature navigator would be:

  1. use "find features" to select all the holes you are interested in
  2. use "group features" to create feature groups containing holes of similar criteria (single one or a combination)
    • same type
    • same size
    • same orientation
    • etc.
  3. use the created feature groups as the geometry for your drilling operations

I would recommend to do extensive reading of the NX documentation, better would be to attend a training where someone experienced shows you the possibilities.

Stefan Pendl, Systemmanager CAx, HAIDLMAIR GmbH
Production: NX10.0.3, VERICUT 8.0, FBM, MRL 3.1.4 | TcUA 10.1 MP7 Patch 0 (10.1.7.0) | TcVis 10.1
Development: VB.NET, Tcl/Tk    Testing: NX11.0 EAP, NX12.0 EAP

How to Get the Most from Your Signature in the Community

Re: Hole Making Questions

Esteemed Contributor
Esteemed Contributor

ducaero wrote:

I also can't find a replacement for engage/retract along tool axis with a distance. That one is very useful on our 5-axis mill. About all I can find is an automatic plane with safe clearance distance which isn't as controllable.


The new drilling operations are now working in the same way as the milling operations, which support clearance cylinder and sphere as well.

Depending on the NX release you are using there have been major improvements on how the avoidance moves are handled.

For this reading the NX documentation is mandatory, especially for the whats new guides of NX starting with NX9 up to the release you are using.

A training by an experienced user would be of benefit too.

As always: post a simple example of your current P2P tool path and we could help in creating a similar drilling tool path.

Stefan Pendl, Systemmanager CAx, HAIDLMAIR GmbH
Production: NX10.0.3, VERICUT 8.0, FBM, MRL 3.1.4 | TcUA 10.1 MP7 Patch 0 (10.1.7.0) | TcVis 10.1
Development: VB.NET, Tcl/Tk    Testing: NX11.0 EAP, NX12.0 EAP

How to Get the Most from Your Signature in the Community

Re: Hole Making Questions

Valued Contributor
Valued Contributor

Thank you for the input and I'm sorry for taking so long to respond. Things can get hectic as we all know. I'm using 10.0.3.5 MP11 currently and I did spend time looking over the documentation. I'm still unable to find hole making more desirable or productive than point to point. I must be missing something. Most likely it's the 20 years of habits I've formed. (I still don't use move object as an example)

 

I've included an example part. The point to point operation took less than a minute to make and will work fine. The hole making took about that long finding the features alone, and the clearance options still don't work for me. I'd appreciate any advise that might make me want to ditch the old and embrace the new.

Re: Hole Making Questions

Siemens Phenom Siemens Phenom
Siemens Phenom

Hi,

 

I don't see a major difference in the time needed to program such an operation for this situation; all holes are identical in diameter and depth and manual geometry selection is simple using all holes on face; and all the holes can all be machined with a single tool axis definition.

 

Using Mousotron to do the comparison, it takes me less than a minute to define both operations:

 

On a much larger set of parts and on average, we have seen a 60% reduction in NC programming time and even a 70% reduction in time needed to update an NC program after a design change when using the new hole making over PTP.  This is typically supported by a 50% reduction in mouse clicks and key strokes and a 75% reduction in mouse travel.

 

Here are just some of the of things that you can't do easily with PTP: 

  • Fast way to program a large amounts of complex holes
  • Little or no manual geometry selection needed through automatic feature recognition 
  • Ability to automatically group holes based on characteristics, size, direction, etc.
  • Keeping track of material removed within a set of operations (automatic RAPTO offset; automatic start position update; etc.)
  • IPW aware hole machining; both at top and bottom of your features
  • Blind Stocks and Through Offsets
  • Full Collision & Gouge Check support
  • Additional cycles for Deep Tapping, Chamfer Milling, Back Countersinking, etc.
  • New capabilities for Sequential drilling and deep hole drilling (automatic handling of intersections)
  • Tracking Points for all drilling tools 
  • Optimized groups
  • Standard NCM

 

Despite all the new capabilities, we do acknowledge that there are still a few special situation where PTP is easier/faster. So we're not taking it away and will continue to allow each and every one of you to decide what works best for you.

 

As for the clearance options, can you ellaborate a bit on your struggles; maybe we can help?

 

NX CAM Development

Tom van 't Erve

Re: Hole Making Questions

Siemens Phenom Siemens Phenom
Siemens Phenom

PTP.pngHoleMaking.png

 

Two missing images from my earlier post.

 

NX CAM Development

Tom van 't Erve

Re: Hole Making Questions

PLM World Member Phenom PLM World Member Phenom
PLM World Member Phenom

I use both PTP and Holemaking operations when they make sense.

 

Unfortunatly Holemaking does not support all the Non Cutting Moves we use like engae and retract when drilling.  I still need to use the PTP operation for this.

 

I have also seen on complex models that it takes longer to generate the hole making operations.

 

I am not too concerned with a couple extra mouse clicks.  My goal is to keet the shop running with consistant output from NX.

John Joyce, Manufacturing Engineer,
Senior Aerospace Connecticut
www.senioraeroct.com
Production: NX10.0.3.5, Vericut 8.0.3
Development: Tcl/Tk
Testing: NX11.0.2.7

Learn online





Solution Information