mazak post issue

[xycnc]

I have a Mazak vtc-300c and am having some issues with the part having major undercuts or gouges from the tool path. I thought it was the machine at first but we looked it over and can't find any backlash issues with it. So we are trying to figure out if it could be a post issue. I was wondering if it could be the fact that when in post out circle it post out as R instead of I and J's. Does anyone out there know if this could cause something like that. I will try to put up some pictures of the part later. It verifys ok on mastercam. But it acts like it looses where its at and at time will gouge in for like a half circle and then be fine in random area's. I was using high speed tool paths Opti core and Hybrid. I dont think its over travel. It seems to do it on Round shapes that is why I was thinking it was maybe a post issue. Any input is greatly appreciated. Thanks in advance.

[Brewster]

Have you tried running it at slower feedrates? i had a similar problem on a Mazak Variaxis. at higher feedrates would undercut posts and gouge walls. When it was ran at slower feedrates, everything was fine. it had something to do with the machine dynamics.

[xycnc]

Here is a picture of the part I hope you can see what im talking about

[xycnc]

I have tried slower speeds. I'm not sure how slow I need to go if thats the case. It seems to do it on round shapes. On one part a 3/16 ball at 35 ipm and it still did it. This job was Al and I ran a 5/16 ball at 85 ipm. Thanks for the response.

[Brewster]

Ok that might not be the same problem, the problem I had went away around 100 ipm. Hopefully some of the more experienced Mastercam guys can be of more assistance.

[JAMMAN]

If you run 2 parts with the same tool, do they turn out identical (divots in the same exact place) or is it more random?

[gcode]

have you tried changing the control def to output i j and k instead of r

[Jack Mitchell]

What was the feedrate?

It looks as if the servos could not keep pace with the programmed feed IMHO

BTW, Gcode is correct about I,J, & K vectoring which makes considerably more code than R values and will slow the interpolation down a bit.

Mazak does make a quality machine tool - you might also float it by Mazak as an open question as well.

 

Best Regards, Jack

[Joe788]

I scrapped a $1000 piece of material because of R instead of IJK. Switch to IJK.

 

Also, are you calling G61.1 for precision contour control?

[Jack Mitchell]

Wow Joe, you came out of this almost hostile, settle down and talk it through so that we can all learn from the question put forth.

PS, no danger or slight intended

 

Best Regards, Jack

[xycnc]

Thanks everyone for your help. G code No i haven't changed post to I,J,K was wondering if it would make a differance before I tried, Joe: No Im not running G61.1 but i have thought about doing that. Jack: The feedrate was 85ipm for finish pass and 185 for rough pass. What picture didn't show was that it too giged the part (rough pass). Jammin I haven't ran this part twice. I had it do it to me on a plastic mold a while back and it did do it kinda in the same place but the second time it did it, it was worse. Im really thinking its the the posting out in R's. Because it seems to do it on Round shapes. I ran a plate to inspect the machine where I cut a circle square and triangle and bored for holes to check it out and everything came back good. But those were all 2d paths. Thanks agian.

[djstedman]

Have run mulltiple Mazaks for a while now.. the amount of 'play' for lack of a better term that Mazak allows when determining a radius is determined by a parameter.. it is ridiculously large..

 

I know on one of our mazaks running r instead of i,j,k you could VISIBLY see the out of round..

 

Swap to i,j,k or figure out the parameter and tweak it..

 

Personally I would just swap to i,j,k we have swapped all of ours to i,j,k since then we have stopped cutting egg shaped holes..

[xycnc]

Alright I guess it sounds like I should change it from R's to IJK's. I will rerun it in a few days and see what it does. Thanks again for input everyone.

[xycnc]

Just wanted to post an update. I changed the post to I,J,K and part looks great! Thats what it was. Thanks everyone for you time.

[Thoob]

I had this happen to me as well before doing a surface contour undercut. I couldn't figure out for the life of me what it was. The part was a very expensive part but we ended up being allowed to feather it in with a grinder. Anyway, it was actually the R output instead of i,j,k. I will also agree with G Code that that is what the issue is. I have changed all my output to i,j,k and haven't looked back since. I too have a Mazak. Its a VTC-250D

 

EDIT - Just noticed your last post, lol. Guess I should read the whole thread before responding.

[GPC_CNC]

I had to change our posts to output in I,J,K for all our Mazaks because of the "egg" shapped holes. Also, Using G61.1 I've found is almost always a good idea. This will keep the machine from cutting corners and true to the programmed tool path. This usually applies to higher feedrates ie 100ipm+. But you can also see it in small or right angle corners that the machine will deviate slightly. G61.1 allows the machine to decelerate into and accelerate out of a corner. There are some parameters that accompany this as well that can tune it in to run smoother. I believe it is an option though.

 

Greg

[Thoob]

I use the Mastercam High Feed option to take care of that. I don't know if it works the same as the G61.1 I have never used that G command. Do you just enter it at the beginning of the program and cancel it at the end? How do you use it?

[djstedman]

Thoob,

 

G61.1 alters how the machine itself performs by increasing the amount it decelerates in corners to better conform to the geometry it was programmed to cut.

 

Using Highfeed in Mastercam alters the code that is being created to do about the same thing ie decel in corners to achieve a more accurate representation of the geometry that was programmed.

 

I beleive G61.1 is an option, as for how G61.1 is used you call it with a K value and you DO include the comma, the lower the K value the more the control will decel into corners, K70 is the default..

 

I think you would need to mess with it on a given machine to see what effect it had on that machine, its effect is controlled by settings in some parameters, im not sure which ones though they might be in the book if the Mazak people were feeling particularly helpful that day .. which knowing Mazak might be iffy lol..

 

G61.1,K40 (turns it on)

 

G61.1,K70 (default setting)

[Joe788]

I rarely alter the K value on any of mine. Just entering "G61.1" is the same as "G61.1,K70"

 

You can call G61.1 any time you want. It doesn't need to be cancelled. The only time you'll want to cancel it is drill cycles, but you don't have to if you don't want to.

 

The machine won't feed faster than 315ipm without G61.1 turned on.

[Thoob]

That is not true. My machine feeds more than 315IPM all the time. i use high feed mills but like I said, never used G61.1, only the Mastercam High Feed option. I have seen others post that same thing about the machine not feeding more than 315. Not sure why people say this unless mine is turned on by default? I have a Mazak VTC250D/50 Fusion 640M control. Is it possible my machine has it on by default internally? It is definitely not on in my G Codes list of activated commands, and I can turn it on with MDI and then it shows it as being on. As soon as I hit reset, it turns off.

[djstedman]

I know we have 4 Smart 430 VTC's they wont feed over 315 without turning on G61.1, I just tested and verified this..

 

We have a bunch of older VTC-160's with the 640 controls.. they will in fact run higher feedrates without the G61.1

 

So its true with the newer machines but not with the older ones from the look of it..

[Thoob]

My machine is 2007. I found out what it was. The parameter M3 is supposed to be set to 8000 which is the max feedrate. 314.8 IPM

Mine for some reason was set to 15000. Hence why I was able to get over 500 IPM without the code. I changed it back to the "default" and am going to start using the G61.1 option as it is the better option for 2 reasons. Less code as the slow downs are internal, and the ramp speeds for the slow downs are specifically set for "your" machine.

What the G61.1 does is change the max feedrate to Parameter M1, which is your max rapid speed, in my case is 30000.

You don't typically need to use the ,K value either. Mazak told me just activating the G61.1 is enough for it to slow down based on your speed and machine. Use the K if you find the machine is still not holding the tolerance you need OR is still hitting the corners too hard.

[Joe788]

That is not true. My machine feeds more than 315IPM all the time. i use high feed mills but like I said, never used G61.1, only the Mastercam High Feed option. I have seen others post that same thing about the machine not feeding more than 315. Not sure why people say this unless mine is turned on by default? I have a Mazak VTC250D/50 Fusion 640M control. Is it possible my machine has it on by default internally? It is definitely not on in my G Codes list of activated commands, and I can turn it on with MDI and then it shows it as being on. As soon as I hit reset, it turns off.

 

Interesting. We've got Fusion, Matrix, Matrix Nexus, and Fusion Nexus controls, and none of them will do a straight feed move above 315ipm without G61.1 active. If it's cutting splines, like dynamic milling it'll creep above that, but I have no idea why.

 

If you just MDI "G01X20.F450.", will it go 450?

 

Edit: Nevermind, didn't see the follow up posts on the 2nd page.

[Thoob]

What is the command to turn G61.1 off?

[djstedman]

G64 is regular cutting mode and will disable G61.1