Spiral Toolpath (Streamline) Question

[KevinW1266]

Good afternoon all,

I'm learning a bit more about the streamline drive for contour milling, and have a question about why my first pass is penetrating the part so much. I'm working on making a toolpath for an incremental forming operation, and to do so I have created a geometry which is the "negative" of the shape I'd like to form, think of it as what you would use as a die if this were a conventional stamping operation, and then specified that the blank is just an offset of 0.150". With this workpiece, and a half inch ball mill tool, I am then trying to mill away this excess from the part wall surface (which will in turn output the toolpath that I need for my blunt tool to do the incremental forming).

I have two issues however that are coming up:

1) The toolpath, when generated, outputs a spiral with the pitch that I am looking for, but the first step is a plunge of roughly 3 times the pitch. I have tinkered around and found that the first step that the software puts in is roughly 1/4 of the tool diameter, which I can then work around by changing the diameter of my part to be formed, but this is quite the hassle. Is there a setting that I am missing which is causing this first jump to be so great? I've added photos below which illustrate this phenomenon also.

2) When all is said and done I post process the toolpath with the canned 3 axis mill (or 3 axis mill TURBO which gives the same problem) and the output G-Code is VERY long. I've cycled through using "Line", "Arc - Parallel to Axis", "Arc - Parallel/Perp to Axis", and even "Nurbs", but each of them give me G-Code that is so long that the CNC controller we use in my lab cannot accept it in a single program. Am I missing something blatantly obvious, or is this just something I'll have to work around as well? I could write a G-Code to do what I want in about 10 lines I think using G2.1 or G3.1 commands, but the program doesn't seem to use these?

Anyway, thanks for any and all help you guys and gals might be able to offer me, and have a great day.

-Kevin

 

[MarioC92705]

Kevin,
for question #1
open the "streamline drive method" dialog box (by clicking on the wrench)
in the "trim and extend" section change the "Start Step" to something like -10

for question #2
change "Motion Output Type" to "Arc-Perp to Tool"
(Machime Control section of the operation dialog box)

Best Regards,

Mario C.

 

[markrief]

#1
Like Mario says, start at -10% or something. The system is looking at the contact point, not the tool tip.

#2
If this is a tapered helix, then there are no arcs, so your output will be linear.
If you want arcs, Try Zlevel Profile, with ramp between levels. That will cut each "level" as an arc, and then ramp down to the next level.

Mark Rief
NX CAM Customer Success
Siemens PLM Software

 

[KevinW1266]

Hey Mario and Mark,

Thank you both for the suggestions! I'll give them a shot in just about an hour and report back what I'm able to do based on your input.

Could I clarify something though with the spiral generation (essentially my 2nd question)? Although I cannot use arcs to simplify the code and limit the number of lines, would that ramping into the next level give me a similar effect? Is there not a way to use G2.1 or G3.1 in NX? Seems like using those commands could severely cut down on the code from where I'm at now.

-Kevin

 

[KevinW1266]

So a bit of an update. As you all suggested, using the starting point as -10% did move the toolpath up to the surface and seems to take care of the issue I had in my first question.

However, the toolpath with the streamline is still roughly 2500 lines (which is 500 more than our CNC controller can handle) so I am going to start working on the ZLevel Profile method to see if this can fix this issue.

Thanks again all!

EDIT: So I've gone to the Z-Level drive method with the ramp between levels set to a very low angle (trying to still get the spiral toolpath) and my lines are up to almost 8000! I really need a strategy to get this spiral toolpath under my 2000 line limit, and I think that the streamline is what I need.

Any suggestions on this? Thanks!

 

[markrief]

The reason for zlevel us to minimize the ramps, and maximize the planar cuts, to produce more arcs.
Did you get circle records for the planar (cyan) cuts?

If you don;t need the continuous, cut, use zlevel with arc engage/retract - this will give you all arcs (see attachment):

N0040 G0 G90 X-.955 Y.1368 S0 M03
N0050 G43 Z.5 H00
N0060 Z.0016
N0070 G1 Z-.0984 F10.
N0080 G3 X-.9791 Y0.0 I.3759 J-.1368
N0090 I.9791 J0.0
N0100 X-.955 Y-.1368 I.4 J0.0
N0110 G1 Z.0016

Another option is to use a chamfer mill and take far fewer cuts.

Mark Rief
NX CAM Customer Success
Siemens PLM Software

 

[KevinW1266]

Hey Mark,

I see what you're saying, and I do get the cyan lines, but I am trying to (in general) eliminate them entirely. I am actually not milling, I'm doing some incremental sheet forming, but using NX to do this type of contour milling which will give me the toolpath I need for the ISF process. For this a spiral is really the key because it keeps the strain rate of the material very constant during forming instead of jumps between discrete levels (like in the Z-Level drive method).

Upon further inspection, the Fadal controller we currently use seems to have a max memory of just under 50 Kbs (roughly 2000 lines), and I am now looking into the possibility of upgrading the memory or using a DNC software to drip in the code line by line. I really do thank you for your help, and if you have any experience with either of these memory workarounds I'd love some insight!

Cheers

 

[cnc07]

Hi,
If you are cutting/driving a constant tapered helical cone shape which seems to be in the images, then only I controller I am aware of requires a single block of code for your entire helical toolpath is FIDIA C20. But it requires the helical output in the cl file. Helical record can be output using MOVARC syntax.
And I am pretty sure it is not possible on a Fadal controller. So either you have to increase the program storage on your machine or use DNC to drip the program.

 

[capnhook]

He's doing some incremental sheet forming, guys......pay attention.

He is NOT milling......put away your chamfer cutters.

Proud Member of the Reality-Based Community..

[green]To the Toolmaker, your nice little cartoon drawing of your glass looks cool, but your solid model sucks. Do you want me to fix it, or are you going to take all week to get it back to me so I can get some work done?[/green]

 

[KevinW1266]

Hey Cnc and Capnhook,

I am indeed doing some incremental forming, and although I think your solution would work I am hopefully going to move on from simple cone shapes into more asymmetric geometries in the near future. So far I've had success with the -10% starting point in the streamline options and I think that as soon as I figure out the drip feeding to my Fadal CNC machine then I should have no issues with the length of the program.

Thanks again everyone!