cancel
Showing results for 
Search instead for 
Did you mean: 

Hole making Tapping feedrate?

Creator
Creator

So I've been using NX cam for a while without any previous training, I've managed to machine some pieces with success, the only thing I can't manage to figure out is the "Tapping" process. The thing is that when I post process the feedrate (f) stays inherted to the value of the "method" you use, even if you use non method you get a random value not depending on the tap. Is there a way the feedrates changes "automatically" according to the spindle speed,tap,Surface speed? some other CAM programs already do this I don't know what I'm doing wrong one thing to now is that if I input the value the feedrate generated by another program it does "correct" the issue, though what I want is a feedrate generated instead not vice versa

Untitled-1.png

11 REPLIES

Re: Hole making Tapping feedrate?

Experimenter
Experimenter

I had a friend who is  well versed in postbuilder to sync this to the pitch of the tap I am using.. so I don't bother setting this... I believe this should be the OTB configuration also..  I have no idea what he did though Smiley Sad .

 

 

 

Re: Hole making Tapping feedrate?

Creator
Creator

You should try to contact him to figure out this Smiley Indifferent

Re: Hole making Tapping feedrate?

Esteemed Contributor
Esteemed Contributor

If you use a *HOLE_MAKING* template "tap" tool (IIRC also for thread mill tool) there is a variable defined in the post "mom_tool_pitch", which is the tool's "pitch" value.

 

Note: in earlier NX versions, "DRILL" template tap tools are NOT set up correctly - you must use the tools from the "hole_making" operation template.  In 10.0.3.5 MP5 it looks like the "pitch" parameter is there (although the picture of the tool is "wrong"), so I don't know if it has been fixed or not.

 

Ken

 

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: Hole making Tapping feedrate?

Genius
Genius

as a workaround, maybe you could consider using Machining Data Library - Tool Machining Data  to automatically set the right speed and feed for the operation.

 

https://youtu.be/NjuH_RPmdiY

 

or, as suggested by Turul and Ken, you can obtain the feedrate during the postprocessing phase, multiplying  $mom_tool_pitch * $mom_spindle_speed (you have to set the correct speed, anyway)

 

ciao

 

Re: Hole making Tapping feedrate?

Pioneer
Pioneer

I just don't understand why this does not work OTB. Once the tap is selected the intention is pretty clear.. This is a tremendous amount of clicking ... It's a neglected area of NX CAM. I think it needs work.

 

 

 

 

Re: Hole making Tapping feedrate?

Esteemed Contributor
Esteemed Contributor

Most modern controllers allow one to specify the pitch in a tapping cycle, so calculation feed rate is not even needed.

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 Tapping feedrate?

Pioneer
Pioneer

Stefan, 

 

I think the point here that this should just work OTB. After you shell out funds for a license you should not have to configure a silly tapping cycle... It should work all 3 ways..  ( IPM, IPR, IPT) ( in inches). These questions should not even come up in this forum. This is supposed to be the most advanced CAM system... Smiley Happy.

Re: Hole making Tapping feedrate?

Esteemed Contributor
Esteemed Contributor

I am of the same opinion, since I had to tweak the post-processor to ignore mmpr and use the pitch instead.

Have you created a problem report at GTAC for this, so that it can be fixed in the future?

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 Tapping feedrate?

Esteemed Contributor
Esteemed Contributor

Note in the post, for cycles, you can specify the feedrate mode as "Auto"

So it outputs xPR ("x" = "I" or "MM") if you specify that in the NX operation, or xPM if you set the operation that way.

Program & tool path -> "Program" tab -> "Machine Tool" group -> "Feedrates" button (in right window) -> (you may have to scroll down) -> Cycle feed rate mode

 

If you want pitch output, you may have to customize (in the post) the tap cycle to always use pitch (assuming it is defined, see below).  If mom_tool_pitch not defined, then post should output a warning and stop/abort.

 

If you do this, in the post's end of path event, I would check to see if the next operation has a tool change, and (if so) do a "catch { unset mom_tool_pitch }" (in case the a later operation uses a "drill" as a "tap" so the *old* tool's pitch ends up being re-used)

 

So, *if the post is set up correctly*, then (in NX) there's NOT a lot of clicking

1) Define tap tool correctly (using tap tool that has pitch)

2) Create tap operation (ignore feedrates unless you do G1 positining to get to hole, between holes, or away from holes - which is not likely as most people use G0 for this)

3) post

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


Learn online





Solution Information