Cancel
Showing results for 
Search instead for 
Did you mean: 

FBM Machining a Hole from Two Sides

Valued Contributor
Valued Contributor

Hello there,

 

I am trying to machine a long Step1 Hole from two sides. Please find the file attached.

 

In MKE, I first used a Dummy Operation to seperate the hole into two shorter Step1 Holes.

Then I used  the DRILLING operation to machine the two holes from two sides. 

 

In NX 8.5, I used to define the positions and directions of the two holes in the Dummy operation (under Machining Knowledge Tab), as follows:

lwf_1.DEPTH = mwf.DEPTH/2

lwf_1.X_ORIENTATION_D = mwf.X_ORIENTATION_D
lwf_1.Y_ORIENTATION_D = mwf.Y_ORIENTATION_D
lwf_1.Z_ORIENTATION_D = mwf.Z_ORIENTATION_D
lwf_1.X_ORIENTATION_L = mwf.X_ORIENTATION_L
lwf_1.Y_ORIENTATION_L = mwf.Y_ORIENTATION_L
lwf_1.Z_ORIENTATION_L = mwf.Z_ORIENTATION_L
lwf_1.X_POSITION = mwf.X_POSITION
lwf_1.Y_POSITION = mwf.Y_POSITION
lwf_1.Z_POSITION = mwf.Z_POSITION

lwf_2.DEPTH = mwf.DEPTH/2

lwf_2.X_ORIENTATION_D = -mwf.X_ORIENTATION_D
lwf_2.Y_ORIENTATION_D = -mwf.Y_ORIENTATION_D
lwf_2.Z_ORIENTATION_D = -mwf.Z_ORIENTATION_D
lwf_2.X_ORIENTATION_L = -mwf.X_ORIENTATION_L
lwf_2.Y_ORIENTATION_L = -mwf.Y_ORIENTATION_L
lwf_2.Z_ORIENTATION_L = -mwf.Z_ORIENTATION_L
lwf_2.X_POSITION = mwf.X_POSITION + mwf.DEPTH*mwf.X_ORIENTATION_D
lwf_2.Y_POSITION = mwf.Y_POSITION + mwf.DEPTH*mwf.Y_ORIENTATION_D
lwf_2.Z_POSITION = mwf.Z_POSITION + mwf.DEPTH*mwf.Z_ORIENTATION_D

and then set the tool going to the corresponding depth in the DRILLING operation.

 

In NX 10, hole_making.DRILLING, it seems that this doesn't work any more, for the geometry now depends on the Machining Area. What I do now is still setting the DEPTH in the Dummy Operation, and in the DRILLING operation, setting the DEPTH in the InProcessFeature Add-on. Besides, reverse the direction of the hole on the bottom side.

 

The questions are:

 

Q1. Is this DEPTH parameter in the Feature Geometry dialog calculated from the tool shoulder or the tool tip? After I did some experiments, it seems that it sometimes includes the tip, sometimes doesn't. When there are two steps in a hole, this DEPTH parameter even becomes unpredictable. In the attached file, I set the DEPTH to be 2.534, but when I verified the path, the distance from the hole top to the tool shoulder is 2.634.

Depth.PNG

 

Q2. Operation S1H_DRL_CLEAR_1 in the attached file is for the bottom side hole. In the Feature Geometry Dialog, I set the IPW as Local. If it works well, this operation should drill the bottom side of the hole. But it doesn't. I had to play a trick to make it correct. I changed the IPW type to None, then changed it back to Local. After that it worked.

 

Thanks,

Kai

15 REPLIES

Re: FBM Machining a Hole from Two Sides

Esteemed Contributor
Esteemed Contributor

We are also migrating our FBM rules from NX 8.5 to NX 10 currently and encountered the same problems, that the new DRILLING operations are not really reliable.

 

The depth in Q1 depends on the depth limit type, through or blind, and the tracking point, tip or shoulder.

 

We haven't found a solution for Q2 either.

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: NX12.0

How to Get the Most from Your Signature in the Community

Re: FBM Machining a Hole from Two Sides

Valued Contributor
Valued Contributor

Hello Stefan, 

 

I have done a bunch of experiments. It seems that the DEPTH is always calculated from the tool shoulder no matter what the tracking point is and whether it is THRU or BLIND.

 

Thanks,

Kai

Re: FBM Machining a Hole from Two Sides

Valued Contributor
Valued Contributor

Thanks. I have solved Q2 by adding the following lines in an Add-on of type "InProcessFeature" in the DRILIING operation. In that way, the position and orientation information can be passed from the Dummy operation to the DRILIING operation.

 

ipf.X_POSITION = mwf.X_POSITION
ipf.Y_POSITION = mwf.Y_POSITION
ipf.Z_POSITION = mwf.Z_POSITION

ipf.X_ORIENTATION_D = mwf.X_ORIENTATION_D
ipf.Y_ORIENTATION_D = mwf.Y_ORIENTATION_D
ipf.Z_ORIENTATION_D = mwf.Z_ORIENTATION_D

 

Kai

Re: FBM Machining a Hole from Two Sides

Esteemed Contributor
Esteemed Contributor

The problem with the InProcessFeature is, that if you add another hole to the process, the changes will not be inherited by the newly added feature.

 

Steps to reproduce:

  1. create two similar FBM features
  2. create the feature process for one feature
  3. create the feature process of the other feature separately with use existing geometry
  4. notice the NXHOLE features below the second FBM feature are not marked as locked as they are in the first FBM feature and there is no overwrite indicator

It seems that only the feature is added to the geometry group and the rules are not checked for manual changes to the InProcessFeature.

In addition any update to the solid geometry will remove the manual edits through the rules.

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: NX12.0

How to Get the Most from Your Signature in the Community

Re: FBM Machining a Hole from Two Sides

Valued Contributor
Valued Contributor

Thanks, Stephan.

 

There is also another problem in setting the DEPTH in a InProcessFeature Add-on. Take the feature VENT_THR in the attached file as an example, operation VT_DRL is for drilling Diameter2. I set the Drilling DEPTH  to be 0.7511 in the Add-on. And in the operation condition, I set 

 

oper.Control_Point_Offset_Type = "InProcessFeature",

 

so that the tool can rapto the bottom of Diameter1 and start to drill Diameter2 from there. However, in the created operation VT_DRL, if you look at the coordinate system, the DEPTH is calculated from top of the hole rather than the bottom of Diameter1, and the drilling starts from the top of the hole.

 

Kai

 

VENT_THRU.PNG

 

 

 

Re: FBM Machining a Hole from Two Sides

Esteemed Contributor
Esteemed Contributor

Yes, we have found that the InProcessFeature add-on breaks the correct behaviour of the in-process-feature update.

It seems that when using the InProcessFeature add-on the system thinks the setting of the control point offset type is "Machining Feature".

 

The transition to the new drilling operations is only an enhancement if you are not using the InProcessFeature add-on, else it is a drawback.

 

On the other hand the rules are now so much simpler, since you don't have to calculate everything for the next rule, you just use the correct machining area in the next rule.

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: NX12.0

How to Get the Most from Your Signature in the Community

Re: FBM Machining a Hole from Two Sides

Esteemed Contributor
Esteemed Contributor

Since I have to change the manual values anyways, I think, I might drop using the InProcessFeature add-on to get more reliable results.

 

I am checking the values I change manually through the rules with a pre-action DLL of the tool path generate menu entry, see the VB.NET source at How do we get the parent CAM.CAMFeature of a CAM.FBM.Feature

If a change is needed that is done through the InProcessFeature add-on, I rename the operation so I can check it with the VB.NET DLL and set the correct values through the DLL.

 

Might be a solution till they get FBM working correctly with the new drilling operations and manual edits.

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: NX12.0

How to Get the Most from Your Signature in the Community

Re: FBM Machining a Hole from Two Sides

Siemens Phenom Siemens Phenom
Siemens Phenom

Hi,

 

A few comments on this discussion thread:

  1. The use of Create Feature Process in combination with Groups Settings " Use Existing" does indeed not set matching parameter overrides and corresponding locks on the additional in-process feature. This is a known limitation/PR.
  2. Overriding parameters on in-process features by using Add-ons in your machining rules works in the same way as manually overriding parameters when you define an operation interactive. The drawback is that these "changes" will be lost after a geometry update. The problem is that the manual overrides lack a clear definition of the user's "intent". We are discussion ways to improve this. One idea is to add a new type of (e.g.) DEPTH intent that is a factor of either the tool diameter of the feature depth. For a pilot hole operation you would then e.g. be able to specify the operation/in-process feature depth as 4.0 time the feature diameter. This would fully specify the depth intent and allow us to retain the intent. The same thing applies to the depth of un-modeled in-process chamfer features; un-modeled thread or the depth of an in-process feature when machining a hole from two sides.
  3. We were able to reproduce Kai's problem with the oper.Control_Point_Offset_Type = "InProcessFeature". This is indeed a software problem. It seems that you cannot yet use the combination of a overwritten depth and oper.Control_Point_Offset_Type = "InProcessFeature" at the same time. I will create a PR for that.

Tom van 't Erve

NX CAM Development

 

Re: FBM Machining a Hole from Two Sides

Esteemed Contributor
Esteemed Contributor

I would suggest the following to make FBM work more reliably with the new drilling operations:

 

  1. add a machining area called FACES_TILTED_TOP, which is of type through hole for spot facing or milling a flat face before drilling
  2. add a depth intent as percentage of modeled hole depth or diameter as already mentioned
  3. add a depth intent for tapping as a percentage of tool diameter and a bottom stock for blind threads
  4. add a depth intent for chamfer milling

If we know how the software works, we can make better suggestions to help you to help us Smiley Wink

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: NX12.0

How to Get the Most from Your Signature in the Community

Learn online





Solution Information