[curiosity22]

Hey G'day folks,

Its me rearing my ugly head again. Ok this is doing my head in - seriously seriously doing my head.... sighhhh..

I am going to attach a file if someone would care to look at it and advise what the @!#$!%#@!@#%!@#% am I doing wrong.

Now if I load this file in Mach it will run fine, I up the anty and increase speed to 250% it moves along appropriately. Z is smashing along at a rate of knots...
Mach will travel left to right in 8/9 seconds. So cutting time is pretty good.

Now load the same blessed file in UCCNC andddddddddddddddddddddd this is where I tear my hair out the little gray withered patch that I have left.
So long as we are traveling in a straight line with z not having to do anything we achieve the same 8/9 seconds.
BUT BUT BUT as soon as Z has something to do well it all goes to the toilet and its a good 30 seconds left to right.
Now I can increase UCCNC to 300% and it will zip on a straight line and back to god so bloody slow soon as Z has to do any work.


Why? heaven help me I've been looking at this for several months now and come back to it every so often.
Balazis gave me a hint with setting under axis setup to increase velocity which dictated if max speed had been achieved when using the % increase.

Kind forum member you know who you are said if I decreased linear and corner error and drop that to .03 rather than it be at .003 under General Setting that should help increase speed as well.

Well bugger it don't help.

So why in Mach I can get speedy speedy speedy and same file UCCNC turtle...

Someone put me out of my misery please.

As a by the by increasing plunge rate seems to do nothing for me either in uccnc

Cheers,
Steve

[FastFarmer]

Now if I load this file in Mach it will run fine, I up the anty and increase speed to 250% it moves along appropriately. Z is smashing along at a rate of knots...
Mach will travel left to right in 8/9 seconds. So cutting time is pretty good.

Now load the same blessed file in UCCNC andddddddddddddddddddddd this is where I tear my hair out the little gray withered patch that I have left.
So long as we are traveling in a straight line with z not having to do anything we achieve the same 8/9 seconds.
BUT BUT BUT as soon as Z has something to do well it all goes to the toilet and its a good 30 seconds left to right.
Now I can increase UCCNC to 300% and it will zip on a straight line and back to god so bloody slow soon as Z has to do any work.

Why? heaven help me I've been looking at this for several months now and come back to it every so often.

And your doing this because; to achieve what?

You "load the same blessed file"?? Did you recompile it with the appropriate post processor?

G-Code an't just gcode that is common to all... All post processors have there own uniqueness, issues, features, and functions.

[curiosity22]

Hey g'day,

Thank you for the reply,

Ok I am doing this to have UCcnc work in if possible the same way at the same rate. I like using UCCNC but I don't want to wait for a Job 8 hours to finish. When I know it can be done in 3 hours.

A good question thank you for asking it - did I recompile it - Answer no... I have been waiting for a reply from Balazis its only been a couple of days but I'm not expecting a reply any time soon so near to Xmas and New Year Im sure he has other things to do in life as well.

The question I did ask him if there was a post processor that was better suited to UCCNC? So far all I have known is as per attached file.

I know that UCCNC and Mach3 interpret the file in a different way. As a matter of fact Balazis did try to answer me in his own way via an email a while ago I will paste his answer.. I believe I understood what he was telling me and looking at the file I feed to UCCNC it should run at max set speed (Z) and it should increase speed with my increasing the % boost. BUT yup always a BUT... something is not right somewhere.

His detailed answer back.. ohh if you have UCCNC and Mach if I might ask you to test it please if you have time...

Regards,
Steve


Subject: Re: increasing speed

Steve,

Thank you for your e-mail.

Well, in the control level of a CNC program like in the UCCNC, Mach3 etc. there is no such thing as plunge rate.
A thing "plunge rate" can be defined in your CAM program, but what that does is that it will place/generate "F" words for your g-code program when the CAM places moves for the Z-axis.

I mean your Z feedrate which you call "plunge rate" is also controlled with the feedrate codes set in the g-code program.
In other words whatever "F" feedrate code is programmed is how fast your Z-axis will travel.
The feedrate "F" always defines the feedrate on the path, so in the case when your machine is plunging, when the Z-axis is the only axis moving then the feedrate of that axis will be the rate of the previously programmed and therefor the currently being active Feedrate value.

So, the plunge rate is controlled in the g-code with the "F' word, to see what exact rate your Z axis will move in the different g-code lines check the F word in your code in the line or before your Z moves.
The F word is modal, which means that as you run your g-code whenever an F word is programmed will be the feedrate used until a new F feedrate word is programmed in the sequence.

Another thing to check is if your Z axis move is defined with G0 or G1 code, because G1 will move with the programmed feedrate, but G0 is rapid move, so if the Z is programmed with G0 then the movement feedrate will be always the maximum speed setup for your axis, in this case the maxium setup for your Z-axis.
Also G0 and G1 codes are modal, so whenever in your code a G0 or G1 or G2 or G3 (these are one modal group) will be active until another code in the same modal group gets programmed.
For example, you have this code:

G0 Z0
Z-10
Z-20

With this code the Z-axis will always move with maximum Z set feedrate, no matter what "F" is programmed, because the G0 gets programmed once and no other first modal code is being executed, so G0 is active for the whole 3 lines of g-code program.

Another example:

F500
G1 Z0
Z-10
Z-20

With this example the Z will always move with a feedrate of 500units per minute, because an F500 is programmed and no more F is defined in the code, so in the next lines the F500 is still the active feedrate value and the code G1 got activated and is still active in all lines of the g-code, because no other codes got programmed (G0, G2 or G3) which could change the activated code in this modal group.
Ofcourse the same is true for the Z-axis as what is true for all other axis that if the programmed feedrate is higher than what feedrate is setup for your axis in the UCCNC setup then the absolute limit will be the setup set feedrate,
in other words the axis will never move faster than the setup set feedrate, no matter if your g-code programs a higher feedrate.

How the feedrate and the G-code modals are handled in the UCCNC is the same as it is defined in the RS274NGC standards book, and it works exactly the same as in any Fanuc type controls, like Mach3, LinuxCNC, etc.

[OlfCNC]

My understanding on the issue you experiencing is that the UCCNC has true deviation control while Mach3 does not.
Mach3 will run whatever path it wants to run on sometimes creating large errors on the workpiece (badly rounding corners for example) while the UCCNC does follow the path with the tolerances you setup which constraint can cause slower running than with "uncontrolled" tolerances like how Mach3 doing it.
With low set tolerances the run will be slower on the complex paths like with wooden reliefs unless you set the tolerances higher in the UCCNC.
You have the choice to set the tolerance higher to run faster with worse results or set tolerances lower to run slower but more precisely, in Mach you do not have this choice, it will make errors on the path what it thinks is OK which can result fast operation in many cases but poor results.

Another idea for you is to increase the acceleration parameter as high as possible that can help a lot on complex paths.

[curiosity22]

My understanding on the issue you experiencing is that the UCCNC has true deviation control while Mach3 does not.
Mach3 will run whatever path it wants to run on sometimes creating large errors on the workpiece (badly rounding corners for example) while the UCCNC does follow the path with the tolerances you setup which constraint can cause slower running than with "uncontrolled" tolerances like how Mach3 doing it.
With low set tolerances the run will be slower on the complex paths like with wooden reliefs unless you set the tolerances higher in the UCCNC.
You have the choice to set the tolerance higher to run faster with worse results or set tolerances lower to run slower but more precisely, in Mach you do not have this choice, it will make errors on the path what it thinks is OK which can result fast operation in many cases but poor results.

Another idea for you is to increase the acceleration parameter as high as possible that can help a lot on complex paths.

Hey Olf G'day,

Thank you for your post,

Ok understood UCCNC has better deviation control, that I understood from Balazs's letter. Which is fine I'm sure for precision work with Metal or materials which are not as forgiving as wood. I have other issues with wood which can be controlled and have to be controlled in other ways. For the type of work that I do, even though precision is required (we don't want a football to look like an acorn) it is more a visual account of the job in the end. I will post the last job I had.

Ok now the tolerances that you are talking about I take are the same ones I mentioned which are found in Configuration/General Settings - Linear error max and Corner error max which in my case are now set to .03 they were set to .003 which is I believe the default setting.

Now I have gone from .003 to .03 which is a reasonable change with no improvement that is noticeable at least. are you suggesting that I should try to take this down further to .3 perhaps? I understand I can trial and error I'm also trying to understand the process. If that is not the control you are referring too where do I find what you are referring too then?

As far as the acceleration parameter is concerned with my earlier correspondence with Balazs I had my acceleration parameters set to 3000 originally when I was testing my CnC build and I believe that was some type of default which was imported from Mach3 profile. I only found out what that did when I couldn't increase the speed of my cnc using the % tool. I have now set that too 14000 plus on all axis. Still even with acceleration set that high - it works great straight line provided there is no pattern. As soon as there is a pattern that goes out the door and the max acceleration I can get is from depending on the bumps say from 300 to peak 1200 in places with the last job I did.

So please note this is not a Mach3 is better than UCCNC or the other way around. What I am trying to achieve is using UCCNC to cut down the job time and finding an effective way of doing that.

This last job I did, job size 490 x 350 x 30mm - no roughing just skimming 8.6mm using a final pass with a 2.5mm ball nose. With the speeds and feeds that I know can be very easily handled by my machine (cruising speed). Job time should be about 1.5 hours. Reality barring mishaps me not paying attention bit breaking etc etc 2 hours start to finish. Mach3 that would be pretty close to the ball mark. UCCNC 6.4 hours. I started and finished the job with UCCNC. Previous job I did was not done using UCCNC.

So if we talked about billable hours, at a measly say $30 per machine hour.. The job using one piece of software or at least having the ability to increase the job speed costs money - more importantly my patience and time. I really do not need to nurse a job for a full 8 hour day when its not needed. At $30 per machine hour count my yawning having a drink reading whats going on in the world and the odd google search I bill for say 3.5 hours. Job cost is $105 I make money person on the receiving end of the bill isn't too bent out of shape either. Conversely at 6.4 hours no yawning time added or google time its $192 machine time - no profit and the person on the other end isn't a happy chappy either.

The type of work I do is not brain surgery its really simple Simon stuff come up with a design that fits, make it look good put some effort in and done. The metal workers I have great admiration for - must be within .0005 a piston in a sleeve can't rub round means round I can understand things being tight. I don't need that - I need a horse that when I stick the boot in - it takes off starts to run and I'm ok with it trying to shake me off and running a little wild .

I have increased and decreased plunge rate and according to Balazs that has no affect on UCCNC at all so moot point there.

How do I get UCCNC to be more a stallion than a lazer beam?

Have a look at my last job like I said not brain surgery simple stuff another rescued piece of timber Red Gum changed from one of those stupid clocks with plastic numbers stuck on the face to a Different stupid clock with some semi naked mermaids and no plastic numbers.

Cheers and thanks to everyone taking time out of their day to put up with my posts, if I'm not being clear enough in what I'm trying to convey please feel free to tell me to pull my head in and breath. I do not mind being told no its impossible to do with X software because.......

Steve

This job did not have to take nearly 7 hours to do from start to finish, remember no roughing straight to final pass.

I'm sure that I'm not the only person to have experienced this but it seems to be obvious that I'm in the dumb and dumber class because I just can not resolve it. If anyone has been there before and knows the way out show mercy and put this old dog to rest.

[mactec54]

curiosity22

Remove these G-codes on line #

N110 Just the G71
N180 G94

Then try it, again, Mach is very forgiving as far as G-Code goes,( it will run anything you throw at it ) where's UCNC is not, the codes you have in there are for a lathe control, G94 is sometimes used for mill if the control accepts it, G71 is Lathe only these could be affecting how your program is running

[curiosity22]

curiosity22

Remove these G-codes on line #

N110 Just the G71
N180 G94

Then try it, again, Mach is very forgiving as far as G-Code goes,( it will run anything you throw at it ) where's UCNC is not, the codes you have in there are for a lathe control, G94 is sometimes used for mill if the control accepts it, G71 is Lathe only these could be affecting how your program is running

Hey Mactec G'day,

Thank you for posting, I will pencil that for the morning to try. Ok lathe and mill dam ok I will try to work out why they are there unless its something generic with the post processor.

Thank you for taking time to look at the file much appreciated.

Off to bed nearly 2 am and I'm not getting smarter.. at least some beauty sleep may do me good.

Will post results once I turn on the machine.

Cheers,
Steve

[mactec54]

Hey Mactec G'day,

Thank you for posting, I will pencil that for the morning to try. Ok lathe and mill dam ok I will try to work out why they are there unless its something generic with the post processor.

Thank you for taking time to look at the file much appreciated.

Off to bed nearly 2 am and I'm not getting smarter.. at least some beauty sleep may do me good.

Will post results once I turn on the machine.

Cheers,
Steve

Yes most Post Processors spit out all kinds of junk that can slow your control down, line numbers are another one,that are not needed, Post Processors are made usually by non machinist, so they just put everything in there, including the kitchen sink, most need to be redone, I don't know why Vectric has not cleaned up there Post Processors

all your axes should be moving at the same feed rate, the way it is programed, did they all appear to move at the same feed rate in Mach

[OlfCNC]

Hey,

I downloaded your gcode and ran some tests to get some results and to help you out. The code looks simple built from lots of small line segments only.
I've tried how fast the UCCNC can run this code (without machine) and detuned the Constant velocity parameters to high values.
Stop angle 100, look ahead lines count 300, linear error 3, linear addition length 20, linear unify lenght 50, corners error 3.
I left the code running to end and it finished in 118minutes.
I had my accelerations on a low level at 200 (forgot to make them higher) so probably could run faster if setting them higher.
This was just to see if UCCNC can finish this job comperably fast as Mach3 and apperantely it can.
I do not know how much error did the software make on the path and how much details it erased using these parameters and I'm not saying to use the mentioned parameters. I did not run this job on a machine, I'm already on holidays away from my machines. but you at least know that it is possible to run faster.

[Jon.N.CNC]

Hey Olf G'day,

Thank you for your post,

Ok understood UCCNC has better deviation control, that I understood from Balazs's letter. Which is fine I'm sure for precision work with Metal or materials which are not as forgiving as wood. I have other issues with wood which can be controlled and have to be controlled in other ways. For the type of work that I do, even though precision is required (we don't want a football to look like an acorn) it is more a visual account of the job in the end. I will post the last job I had.

Ok now the tolerances that you are talking about I take are the same ones I mentioned which are found in Configuration/General Settings - Linear error max and Corner error max which in my case are now set to .03 they were set to .003 which is I believe the default setting.

Now I have gone from .003 to .03 which is a reasonable change with no improvement that is noticeable at least. are you suggesting that I should try to take this down further to .3 perhaps? I understand I can trial and error I'm also trying to understand the process. If that is not the control you are referring too where do I find what you are referring too then?

As far as the acceleration parameter is concerned with my earlier correspondence with Balazs I had my acceleration parameters set to 3000 originally when I was testing my CnC build and I believe that was some type of default which was imported from Mach3 profile. I only found out what that did when I couldn't increase the speed of my cnc using the % tool. I have now set that too 14000 plus on all axis. Still even with acceleration set that high - it works great straight line provided there is no pattern. As soon as there is a pattern that goes out the door and the max acceleration I can get is from depending on the bumps say from 300 to peak 1200 in places with the last job I did.

So please note this is not a Mach3 is better than UCCNC or the other way around. What I am trying to achieve is using UCCNC to cut down the job time and finding an effective way of doing that.

This last job I did, job size 490 x 350 x 30mm - no roughing just skimming 8.6mm using a final pass with a 2.5mm ball nose. With the speeds and feeds that I know can be very easily handled by my machine (cruising speed). Job time should be about 1.5 hours. Reality barring mishaps me not paying attention bit breaking etc etc 2 hours start to finish. Mach3 that would be pretty close to the ball mark. UCCNC 6.4 hours. I started and finished the job with UCCNC. Previous job I did was not done using UCCNC.

So if we talked about billable hours, at a measly say $30 per machine hour.. The job using one piece of software or at least having the ability to increase the job speed costs money - more importantly my patience and time. I really do not need to nurse a job for a full 8 hour day when its not needed. At $30 per machine hour count my yawning having a drink reading whats going on in the world and the odd google search I bill for say 3.5 hours. Job cost is $105 I make money person on the receiving end of the bill isn't too bent out of shape either. Conversely at 6.4 hours no yawning time added or google time its $192 machine time - no profit and the person on the other end isn't a happy chappy either.

The type of work I do is not brain surgery its really simple Simon stuff come up with a design that fits, make it look good put some effort in and done. The metal workers I have great admiration for - must be within .0005 a piston in a sleeve can't rub round means round I can understand things being tight. I don't need that - I need a horse that when I stick the boot in - it takes off starts to run and I'm ok with it trying to shake me off and running a little wild .

I have increased and decreased plunge rate and according to Balazs that has no affect on UCCNC at all so moot point there.

How do I get UCCNC to be more a stallion than a lazer beam?

Have a look at my last job like I said not brain surgery simple stuff another rescued piece of timber Red Gum changed from one of those stupid clocks with plastic numbers stuck on the face to a Different stupid clock with some semi naked mermaids and no plastic numbers.

Cheers and thanks to everyone taking time out of their day to put up with my posts, if I'm not being clear enough in what I'm trying to convey please feel free to tell me to pull my head in and breath. I do not mind being told no its impossible to do with X software because.......

Steve

This job did not have to take nearly 7 hours to do from start to finish, remember no roughing straight to final pass.

I'm sure that I'm not the only person to have experienced this but it seems to be obvious that I'm in the dumb and dumber class because I just can not resolve it. If anyone has been there before and knows the way out show mercy and put this old dog to rest.

I too have migrated to uccnc but not had this issue myself.

3000 acceleration? do you mean volocity? You haven't confused the two? 3000ps/ps is crazy, and I think impossible.

Also does the z jog at the set volocity?

[vmax549]

First question are Both controllers set with the exact same parameters for the axiss XYZ ??

What controller is being used with the Mach3 version LPT ?? other ?? OR are you using the same controller for both ??

What kernal speed are you using for each one ?? the same ??

(;-) TP

[curiosity22]

Hey Vmax G'day,

Using Gecko G540 4 axis - Same parameters for X and Y which also has a slave A - Z being screw is different to the other 3 which are helical coil rack and pinion.
Same kernel speed, UC100 controller.

To the best of my ability both software programs being different from each other everything else is set the same.

I was going to start up another job and test some more settings to see whats what.
I can't believe how stupid I must be because there's not much there to change or fiddle with its not like there are pages and pages of settings.

Unfortunately I got some bad news while typing this that a very good friend of mine has had a relapse of cancer and it is terminal, so my pissy issues will be left for a few days while I go see my mate.

Cheers,
Steve

and thanks for replying to this post vmax its much appreciated.

[ger21]

All velocities and accelerations are the same?

[RCaffin]

So long as we are traveling in a straight line with z not having to do anything we achieve the same 8/9 seconds.
BUT BUT BUT as soon as Z has something to do well it all goes to the toilet and its a good 30 seconds left to right.

I do not run UCCNC, but it's not that much different from Mach3.
Since Mach3 can run your program satisfactorily, we can say there is no problem with your hardware.

From what you are describing, it sounds as though the X and Y axes are being slowed down to match the best performance the UCCNC SW can deliver to the Z axis. This does not mean the UCCNC SW is faulty, just that the configuration file is slightly stuffed. I suggest that the Z axis top speed as set in the configuration file is missing a zero - or maybe the Z axis acceleration is. This will only become apparent when there is Z axis movement simultaneous with X and/or Y movement.

Does this mean that your machine is actually running to spec as defined by the config file? Yes. Does this mean I can duplicate your symptoms in Mach3? Yes, certainly. Been there, done that, had to rebuild the XML config file from scratch when the computer died rather badly.

So, sit down and start tweaking the config file. If I am right, that is the only way of fixing your problem.

Cheers
Roger

[OlfCNC]

I think the issue is simpler than that. The code curiosity uploaded has XY straight scan like moves while the Z moves are kind of sharp.

Imagine one simple square shape to cut.
With Mach3 that will cut with the tool moving around the shape with the tool rounding the corners with undefined radiuses.
My experience is that the radiuses will be acceleration parameter dependent and ofcourse speed. The lower the acceleration the larger the radiuses will be.
I've studied this behaviour of Mach a lot when setting up my plasma machine.

With UCCNC the same will cut with the tool moving around the shape with the tool rounding the corners, but all the radiuses will have a max. size you set in the setup.
The slower the acceleration the larger the radiuses will be but the radiuses will never be larger than what you setup.

It's simple to see that if Mach3 will make large enough radiuses while if the UCCNC has a setup limit on that then Mach3 will finish this job faster because the shape will be less square, more rounded,
less acceleration and decceleration is needed and shorter is the path.
The same is with complex paths, the UCCNC can be tuned to make less or more errors on the workpiece and the low set error can limit how fast the job will finish.
I ran the code of curiosity22 with setting the constant velocity parameters high enough that the uccnc ran similar fast as mach3, but with these settings it will probably erase more details of the relief than if the CV parameters are set low.

[ger21]

As Olf said, I think you need to look at the Configuration > General Settings page and look at pages 29 and 30 in the manual. I would think that your CV mode settings are what is slowing you down.

[curiosity22]

I do not run UCCNC, but it's not that much different from Mach3.
Since Mach3 can run your program satisfactorily, we can say there is no problem with your hardware.

This does not mean the UCCNC SW is faulty, just that the configuration file is slightly stuffed.
So, sit down and start tweaking the config file. If I am right, that is the only way of fixing your problem.

Cheers
Roger

Hey Roger G'day,

Thank you for your post, please note under no circumstances am I saying that UCCNC is faulty. It is working as intended I am sure of that. It's more a case of I'm just dumb and not understanding what to tweak to make it work the way I need it too.

Cheers,
Steve

[curiosity22]

Hey,

I downloaded your gcode and ran some tests to get some results and to help you out. The code looks simple built from lots of small line segments only.
I've tried how fast the UCCNC can run this code (without machine) and detuned the Constant velocity parameters to high values.
Stop angle 100, look ahead lines count 300, linear error 3, linear addition length 20, linear unify lenght 50, corners error 3.
I left the code running to end and it finished in 118minutes.
I had my accelerations on a low level at 200 (forgot to make them higher) so probably could run faster if setting them higher.
This was just to see if UCCNC can finish this job comperably fast as Mach3 and apperantely it can.
I do not know how much error did the software make on the path and how much details it erased using these parameters and I'm not saying to use the mentioned parameters. I did not run this job on a machine, I'm already on holidays away from my machines. but you at least know that it is possible to run faster.

Olf G'day,

Thank you for those numbers, I have UCCNC now operating at similar speed to Mach as well.
I know now where I was falling over, the mistake I was making. When I was reading the manual it was my mistake for not undertanding what was written. It is a little bit of English to French translation problem on my part.. (I know Balazs isnt French) - The English chopping a tree down then chopping it up.. Well once you have chopped it down how do you chop it up...

In the Manual it says,
Linear error max.: This parameter sets the maximal linear error for the interpolator and works in constant velocity mode only. "The higher the parameter is set in most cases the faster the job will finish", because the interpolator will shorten the motion path as much as possible with the linear error setting.

Well I literally understood that as setting is .003 make it higher... .0003 to .00003 of course stupid yes..... Higher meant as in a higher value... .003 to .3 ----- .3 being the higher value.
So I was totally doing things backwards, the lowest I went was .03 which was too slow as well. Olf .3 solved my issue and the numbers that you gave cut machine time down by 400%....... I think I have a better chance of understanding and working out what linear addition length and linear unify length is all about now as well.

Thank you Thank you Thank you Thank you Thank you Thank you Thank you Thank you Thank you Thank you Thank you Thank you Thank you Thank you Thank you Thank you Thank you

With these settings I know I will loose some minor details for sure, I have seen how much loose of detail occurs with two jobs which are the same between Mach and UCCnC but on somethings that loose of detail is OK as most of the work that I do is not made for close scrutiny and made for a viewing distance of 6ft to across the room. Which means the .5mm detail is lost to vision anyway.

I apologise guys for not answering sooner but I had to spend some time with my mate who is well rather lost at the moment as you can all imagine. I know the majority of you guys work in metal as well so my apology for bringing up stuff to do with wood as well.

I will answer the rest of the posts that I missed and thank everyone for the courtesy of their reply's.

Cheers,
Steve

[curiosity22]

As Olf said, I think you need to look at the Configuration > General Settings page and look at pages 29 and 30 in the manual. I would think that your CV mode settings are what is slowing you down.

Ger G'day and thanks for your post,

Olf was right on the money mate, I have looked at those pages many many many times and I was just reading it and understanding it as per my post backwards. Going to the right of the decimal point is not higher but lower..


Cheers,
Steve

[curiosity22]

I too have migrated to uccnc but not had this issue myself.

3000 acceleration? do you mean volocity? You haven't confused the two? 3000ps/ps is crazy, and I think impossible.

Also does the z jog at the set volocity?

Jon g'day,

Yes I did mean Velocity... Z set at the same velocity.

I think why I was having so many issues apart from not being so smart is due to my importing the Mach XML settings. What I should have done was started from scratch and gone through each setting and learning properly what each did rather than looking for the quick fix.

Cheers,
Steve