does high speed machining in machine conflict with high speed tool paths

[connormac]

I have my post's (8) set up so turn on high speed machining (G05.1 Q1)always unless it is drilling. I have been told that now that we are really starting to use 2d high speed tool paths that it is taking the 2d high speed tool paths operations longer with high speed machining turned on in machine (G05.1 Q1). I can go back and put in a mis. integer.( ?? ) and then we will have to manually turn it on for each path. Which is correct?

 

Hope this makes since.

Thanks for looking

Connormac

[Guest]

Hi Kyle, hope things are going well.

 

Yes, you're going to need to add an additional check, an MI is a good idea, so you have operation level control instead of just letting it run on everything.

 

I might just make it an mi level option, if mi9, highspeed codes

 

You'll just have to now remember to set it for each op.

 

You might keep in the post that if a drill cycle, it woun't output it, so you can't make that mistake with an mi.

 

As far as "if it conflicts" I can see where it might depending the machines hi speed funtions ability, it will see all the arcs and constantly reading ahead for smaller arcs, likely leading it to slow down more than it needs to. Again though it may well be machine specific too

[connormac]

Hey John,

Things are going Ok, thanks. Just trying to learn about high speed tool paths. Got a new programmer here and he uses them alot so I have to learn so I can improve my programs. Thanks for the answer I will fix it. Just wanted to make sure before going to all the work.

 

Thanks again

 

Kyle

[SledGeek]

As far as "if it conflicts" I can see where it might depending the machines hi speed funtions ability, it will see all the arcs and constantly reading ahead for smaller arcs, likely leading it to slow down more than it needs to. Again though it may well be machine specific too

 

Yup. See it on mine under certain circumstances with G5.1. I have the AI APC so it's pretty basic control. I have found tht you need to do a little R&D with the highspeeds. I'm finding out that there are certain ones in 2D and 3D that will slow ya down a bit. Not worth turning off for me cuz it leads to jerking. But finding the best suited path for geometry happens quite often. Thank god there not huge parts.....

For instance using Surf. Area Clearance instead of OptiArea cuz it generates less arcs for this particular geom. While opti would actually cut it a bit faster in backplot, on the machine the area cuts it faster......

[NOTW Programmer]

You could pull up an MPMASTER post and see the modifications needed in order for the mi to be used as a switch.

     if mr1$ = 2, #AI-NANO 2, AI(nano)CC output (Artificial Intelligence Contour Control) - G05.1 Q1
       [
       pbld, n$, *sg49, e$                                            #Must be in G49 and remain before G43
       if ipr_type > 1, ipr_type = 0                                  #Must be in G94
       pbld, n$, sgfeed, e$
       pbld, n$, "G05.1", "Q1", [if mr2$, "R", no_spc$, *mr2$], e$    #Mr2 gives accel/decel value/coefficient, usually R or P
       mr1_flg = 2
       ]

And also modify the mr1 description in the CD to match the POST description if you'd like.

 

JP - Is there a way for the RPM during a 2D HSTP for entry be output from the begining, when I use a helix I get the HS RPM first then when it starts the Helix the entry RPM and once its at depth the Dwell then HS RPM again.

 

T8 M6( 1/2 CB GUHRING VARIEM  TOOL - 8)
( PKT RGH )
( OP1 )
A0.
G0 G90 S4750 M3 E1 X1.7517 Y1.8387
G43 Z2. H8 D8 M7
Z.1
G1 Z.05 F100.
S1910 M3
X1.7779 Y1.8168 Z.0488 F25.

 

The problem with this is that it speeds up, stops, changes gears, turns on spindle again, then cuts.

[Tony35]

i use G5 P10000 and its on all the time except for drilling

helps prevent jerking of the machine

[john316]

Depending on what kind of machines you have you may need the G05.1 to keep the machine from skipping corner radiuses, etc. The only difference will be the tolerance (Q value). You can find the tolerance level settings in your machine manual.

 

On one of our 5-axis high-speed machines that has different levels of accuracy I used mr3 to inseret the accuracy code I want. This machine uses m-codes for tha callout so I set it up like this.

 

# mr3 - Used for Machinining Tolerance codes in Toolpath.

# 0=M155(Finishing, Default)

# 0=M156(Roughing, Automatically Outputs if Leaving Stock on Part)

# 1=M157(High Accuracy Finishing)

# 2=M159(5-Axis Simultaneous) uses cuttype for output

 

If I leave it at zero it defaults as shown by reading the stock remaining. There is a drawback to that in that if I want to finish with a different stock than sero it gives me the roughing code. I just have to remember that whenI make code. I also have to remember to change the mr3 to 1 or 2 if I want the high accuracy callout but I usually wait until I'm done and select all toolpaths that I want changed and use the "edit common parameters" function.

[huskermcdoogle]

Hey guys,

 

I am using G05 P10000 on a Mori Horizontal, and I don't think that I have the option to change the tolerance level on the fly. Sometimes it is a bit ridiculous how much it slows down the machine, especially when using OptiRough, Dynamic Mill, or Peel Mill. Is this something that the end user could set up in the control by programming parameter changes in custom M codes to change the values to speed things up? Then default them back to factory settings during your toolchange macro, so you don't mess us any old programs?

 

Another questions related to this... Can you speed things up by getting the machine servos tuned? Anyone care to comment about this?

 

This a time comparison on my last project from tool to tool how much longer it took to run in the machine vs mastercam time.

 

Tool# Actual MCam Delta

40 0:00:50 0:00:01 0:00:49

156 0:01:40 0:01:29 0:00:11

3 0:00:24 0:00:04 0:00:20

62 0:00:23 0:00:09 0:00:14

95 0:05:48 0:05:23 0:00:25

12 0:08:30 0:06:00 0:02:30

174 0:25:33 0:21:36 0:03:58

175 0:32:51 0:26:17 0:06:34

176 1:01:37 0:49:59 0:11:38

76 0:03:07 0:02:37 0:00:30

177 0:03:51 0:02:33 0:01:18

178 0:18:07 0:11:17 0:06:50

 

 

 

 

Thanks,

 

Husker

[connormac]

Hey All

 

Thanks for the replys. I have everything fixed except... I was told that I had to have the

G49

G05.1 Q1

 

Before my G43 line.

 

But how do you do this if you use the same tool to do a 2d high speed tool path then use the same tool to finish. The only way I can figure is to do forced tool change. Or use a diffrent tool. So close but not there yet.

 

Thanks

Connormac

[Guest CNC Apps Guy 1]

MPMaster outputs the HSM codes in their proper location and format. I'd start with that. This has been covered ad nauseum here. Do a search for G5.1...

 

To answer the original topic question, the two do not conflict and have nothing to do with each other. HSM toolpaths have to do with an approach to material removal, HSM codes in the machine have to do with Acc/Dec and code processing. Some builders have built in algorithms that prefer TONS of point to point data, others have no such preference.

[YoDoug®]

MPMaster outputs the HSM codes in their proper location and format. I'd start with that. This has been covered ad nauseum here. Do a search for G5.1...

 

 

We have a Bridgeport GX1300 with Fanuc Oi-MC here that the standard MPmaster X5 post will cause a crash if you run back to back toolpaths with the high speed (G05.1) triggered from the toolpath. It cancels the TLO with a G49 in between the tool paths causing the machine to move the Z. I have been so busy that I have not found the time to see if there is a post tweak or possibly a machine parameter that will change its behavior on a G49.

 

 

 

[Guest CNC Apps Guy 1]

We have a Bridgeport GX1300 with Fanuc Oi-MC here that the standard MPmaster X5 post will cause a crash if you run back to back toolpaths with the high speed (G05.1) triggered from the toolpath. It cancels the TLO with a G49 in between the tool paths causing the machine to move the Z. I have been so busy that I have not found the time to see if there is a post tweak or possibly a machine parameter that will change its behavior on a G49.

 

 

 

SO it cancels HS between ops? That's not right... Wondering if I made that change to my MPMaster posts... :headscratch: My post does not issue a G49 on null tool changes UNLESS I zero return Z as well.

 

I have an machien with an 0i-MD here. I'll do some testing to see what I can get away with and let you know. I still have to install it so it's will probably be tomorrow, but I'll check it out. There probably is a parameter that dictates behaviour on a G49 call though.

[Joe788]

We have a Bridgeport GX1300 with Fanuc Oi-MC here that the standard MPmaster X5 post will cause a crash if you run back to back toolpaths with the high speed (G05.1) triggered from the toolpath. It cancels the TLO with a G49 in between the tool paths causing the machine to move the Z. I have been so busy that I have not found the time to see if there is a post tweak or possibly a machine parameter that will change its behavior on a G49.

 

Yeah, that is a disaster waiting to happen. The Mazak HSM implementation in MPMaster are incorrect as well, other than where they are activated.

[huskermcdoogle]

Yeah, that is a disaster waiting to happen. The Mazak HSM implementation in MPMaster are incorrect as well, other than where they are activated.

 

 

Disaster that has happened with a 5" PCD Facemill..... Lets just say there wasn't much warning, I had turned it on in a proven program by mistake on that tool.....

 

Yeah I took out the G49 as it really doesn't need to be in the post. I do it in the tool change cycle. If it were to be in the post I would put it in the pretract statement, on retract between b-axis moves, which would pretty much make sure that G43 was reapplied correct?

 

Husker

[Guest CNC Apps Guy 1]

Yeah I took out the G49 as it really doesn't need to be in the post unless you're using AI-NANO/AICC. I do it in the tool change cycle. If it were to be in the post I would put it in the pretract statement, on retract between b-axis moves, which would pretty much make sure that G43 was reapplied correct?

 

Husker

FIssed and sounds about right.

[Newbeeee™]

We have a Bridgeport GX1300 with Fanuc Oi-MC here that the standard MPmaster X5 post will cause a crash if you run back to back toolpaths with the high speed (G05.1) triggered from the toolpath. It cancels the TLO with a G49 in between the tool paths causing the machine to move the Z. I have been so busy that I have not found the time to see if there is a post tweak or possibly a machine parameter that will change its behavior on a G49.

I would do the post mod first and formost. You really don't want a G49 buried 'hidden' in a program, even if you do find and change a machine control parameter to make it run ok.

The next machine the prog runs on may not have that parameter changed...

[huskermcdoogle]

FIssed and sounds about right.

 

G49 just needs to be active for G05.1 Q1 to be called. You do not need to call it as G49; G05.1 Q1; Which is also the call for SHPCC on older 16i controls.

Husker

[Cannon]

We have a Bridgeport GX1300 with Fanuc Oi-MC here that the standard MPmaster X5 post will cause a crash if you run back to back toolpaths with the high speed (G05.1) triggered from the toolpath. It cancels the TLO with a G49 in between the tool paths causing the machine to move the Z. I have been so busy that I have not found the time to see if there is a post tweak or possibly a machine parameter that will change its behavior on a G49.

 

There was/is a problem in MPMaster post that did that and it only did it when you used G05.1 code. Someone also posted a post mod that fixed it but I cannot find it anymore.

[Cannon]

Ok, I found the post My link

[SledGeek]

We have a Bridgeport GX1300 with Fanuc Oi-MC here that the standard MPmaster X5 post will cause a crash if you run back to back toolpaths with the high speed (G05.1) triggered from the toolpath. It cancels the TLO with a G49 in between the tool paths causing the machine to move the Z. I have been so busy that I have not found the time to see if there is a post tweak or possibly a machine parameter that will change its behavior on a G49.

 

 

Have Oi-MC\bridgeport here and not getting that. Used old post from 9(updated) as well as the X5 MPMaster post updated to X6 and don't have that issue. Try not using the G49 ,try G91 G28 Z0 followed by G28 X0 Y0, then T--- M6. The only time we use G49 is manually when the program is stopped in the middle before the next tool callout.

Might be a parameter somewhere in toollength comp ?

[YoDoug®]

Ok, I found the post My link

Tried Matts post fix and so far it looks great. Thanks.

[Guest CNC Apps Guy 1]

G49 just needs to be active for G05.1 Q1 to be called. You do not need to call it as G49; G05.1 Q1; Which is also the call for SHPCC on older 16i controls.

Husker

Actually, you can issue the first G5.1Q1 and then cancel it, but until you execute a G49, it will not allow you to execute another G5.1Q.