Does anyone have any experience with post processing or controller knowledge for the Fanuc 16m using RTCP with G43.1 output?

As I understand it, (use of RTCP with G43.1) the program posted machine file output is to be in tool tip coordinate along with rotary A and B values and linear feedrates. The controller uses stored gagelength offset values, and the stored pivot point location value, and does the final trig calculation processing for the pivot point location on the fly. I also understand that it is suppose to use the linear feedrate values and calculate the inverse time feedrates internally when making linear/rotary moves.

I have been experiencing feedrate problems on rotary moves. They are too slow like the controller needs inverse time (min) feedrates in G93 mode.

Any help would be appreciated. Thanks

Dave

I don't know. The controller probably uses some abritary value like 1.0 like any other CAM program uses but without the luxuary featrue of Fedrat/lenght,n  like we have in most CAM post processing software.

GOOD DOCS Bryan

This looks like what I mean...but not sure

3)?Make sure to set length compensation using the gauge line as the datum line for length. This will effect the speed control.


Example Settings of Alignment and length compensation values when using G43.4
??Machine Control point (Rotational Center)
??Tooling Tool Length
??NC Parameter No.19666 (F-15 I = No. 7548)
???Set Value = Actual Pivot Distance
??Post Processor Set Value
???Set Value=0.000
??G43.4 Tool Length Compensation Value
???Set Value = Tooling Tool Length
??G54 Origin of Z Axis Alignment height.
???Gauge Line Position (Where Tool Length =0.000mm)

Bryan

Thanks for the info.

What do you think might be causing my feedrate problem? Just for example I am maching the sides of a part at 40ipm up to a cross rib that is on a 12 degree angle. The tool travels at 40ipm in xyz linear motion but when it starts the AB rotary motion (feed still at 40ipm) to become tangent to the 12 degree rib it rotates real slow like maybe the Max. degrees/ min value is set real low. Is there a setting in the controller to control MAXDPM? Maybe that is the problem?

On a Fanuc, G43.1 needs inverse time feed rates, while G43.4 doesn't.

I think...

Cheers.

I have never had to use inverse time for either type of compensation. I'm pretty sure you're wrong Sporter. At least on the Fanuc 18i control.  The sample programs above from Fanuc do not contain G93 inverse time....I can dig up some old programs in the morning, and I'm sure I won't find inverse time in them.  No complaints from my customer so far.

Just in the last 6 months, I have setup about 8 different 5 axis machines using the Fanuc controller running under RTCP using the G43.x codes.

I use FEDRAT/INVERS,AUTO and MODE/TLVEC,ON to handle all this very easily..

with kind regards
Deepak Manuel
Dassault Systemes

Sounds cool Deepak, so your post automatically outputs a feedrate value for a set distance from the tool point I take it...I'm not an expert on controls, but I would assume there must be a parameter for the distance along the tool axis to gage the automatic inverse time feedrate as if it was computed at the exact tip of the tool, it could be infinite when fanning about the tool tip. I'd assume there is a parameter in the control to set that value....might be the problem that Blotz is having.

My post uses SET/CUTDP,.5 for instance if I want to compute feedrate at .500 up from the tool tip which is what I usually use as default for 4 or 5 axis fanning. I guess you set up ICAM to use the statements you posted above. ICAM sounds really good...I wish I had time to manage post-processors...or I'd probably buy a copy....for now I just buy generic Fortran based posts as I need them, but they come with configuration files so I can set them up for controls that are basically similar.

Deepak

Thanks for the posting. I am assuming from your post statements that you are using the ICAM post processor QUEST for post development and GENER for posting. Reading the manual on RTCP which is turned on by MODE/TLVEC,ON (and outputting G43.1) it says that only linear feedrates are output because the controller is supposed to do the rotary feed calculation on the fly. The ICAM manual says under RTCP features GENER will "Ignore the effects of RTCP enabled rotary axis on the tool feed calculations."

Since I don't know what is correct, Are you outputing G93 and inverse feedrate numbers in your machine file read by the controller? From what I am told and have heard in this forum that they are not used with G43.1.

Thanks again for all your help. It has been very good.

Bryan and Sporter

Thanks for your input here in the forum. But I am confused from your conflicting postings. I have very limited experience with the use of the Fanuc 16m and G43.1, all though I have experience with the Seimens 840D which uses the RTCP command TRAORI and it works very well with only XYZAB OR AC and G94 linear feedrates. The Seimens 840D does not use G93 inverse time feedrates either.  The machine I am programming for is an OKK 5axis (AB head) single spindle mill and the controller I am programming for is the Fanuc 16m. 

I am new at this company. The programmers here only use G43.1. without G93. But I am still having feedrate problems. I have read the Fanuc 16mc, 18mc, 160mc, 180mc manual but it doesn't talk about this problem in detail.

I've always been led to believe G43.1 needs inverse time feed get accurate feed rates while G43.4 doesn’t. Using G43.1, the post needs to know the pivot distance and the tool length to work out the G93 feedrates, while the control needs to know the pivot distance and tool length to work out the head position. But I have never tested it to know for a fact.

Using G43.4, the control takes care of both. Saying all that, I have used G43.1 without G93 feedrates myself with no real problems. (to the untrained eye, if the heads still moving, it looks OK. )

Looking in my Fanuc 16/18 manual under G43.4, it does say –

 “When Linear interpolation (G01) is specified, the feedrate is controlled so that the tool tip centre moves at a specified feedrate”

 
I can’t find anything like that under G43.1. But Fanuc manuals are as clear as mud. Maybe you can add 200mm to the tool length at the control, dry run it and see if it affects the feedrate of the machine?

G43.1 and G43.4 are available on both the 16 and 18 fanuc controls. And G05 P10000 is just High Precision Contour Control, nowt to do with G43.1 or G43.4

Cheers.

Bryan

Thanks for the responces. I appreciate them very much.

I didn't know that, it would explain a few things.

I've programmed for a machine that only had G43.1 and not G43.4. We programmed to tool tip using G41.1, and I'd assumed it was a poor mans G43.4 and needed G93 feedrates, which do the trick. But we were never too far off just using normal feedrates either. 

Funnily enough, we just upgraded an older machine here with G43.4 to match a new machine we have. I just need to find the parameter thats stop the Z coming down by the tool length on G49 and I'll be laughing.

Cheers.