CTX Gamma 1250 CNC code parameter

[rusty.ross]

Just a quick question that maybe one of you guys might be able to help me with. My co-worker and I are banging our heads trying to figure out what this machine is supposed to be doing. We bought a "turnkey" Mill turn software from Mastercam that hasn't worked since day 1. We have the code that Mastercam outputs but that is where we have hit a wall. Both Mastercam and DMG Mori have no idea what's going on, nor have they been at the machine to see it for themselves. We are at our wits end!

For starters, the output has everything in one file, including the subs which coming from another siemens control I know they should be separated, right?? Second is there a parameter or something that we are missing to take this machine out of shop turn and program/run it like a FANUC control? I know it's a siemens but just plain old G-code. We are loading the code into channel 1 but it's wanting something in channel 2, I think. Both him and I are not versed well on this machine, so we feel like we're on an island just waiting out the storm lol.

 

This machine has the CELOS front end and I have read you can disable the CELOS? Is that what is needed to run our own code?

TIA

[gcode]

Rusty

Those look like pretty cool machines. 

CTX Gamma

I can't help you with your problem, but I have moved your post to the Industrial Forum, where it will get more eyeballs.

I'm sure there is someone here who can help.

Which model did you buy?

[rusty.ross]

35 minutes ago, gcode said:

Rusty

Those look like pretty cool machines. 

CTX Gamma

I can't help you with your problem, but I have moved your post to the Industrial Forum, where it will get more eyeballs.

I'm sure there is someone here who can help.

Which model did you buy?

Thanks, but we don't like them lol

 

We have (4) of the same machine, dual spindle dual turrets with live tooling. 

[Aaron Eberhard]

I don't have a CTX handy, but I just did some MT programming for an NTX (to be honest, I'm not sure what the difference is ).  

When I posted out the code, it will generate a "-upper" and "-lower" version.  For example, here's a file 0009 posted:

 

Unfortunately, that's where my knowledge of 'em ends, as I never actually ran one.  From what I can tell it was out being output correctly, though, the setup guy/operator I was working with seemed happy enough?

If you could post a sample file (zip2go so we have the machine def), we might be able to help specifically.

 

You may already know this, but it chooses the "stream" to output based on the individual toolpaths' "Axis Combination" selection, i.e.:

So anything happening on the lower stream has to be programmed to Lower Left/Right.    I've seen a lot of old school lathe guys getting into MT forget to check this, as they just set everything up to the Upper Left all their lives.

[scottm085]

We have two CTX Beta TC 4A's and they have been nothing short of a pain to program. Ours have Siemens controllers that read Gildemeister structure, so maybe not the same situation you are in. What I do know is that for ours to run the controller needs code in both channels, even if you are only using one channel. For instance, if we are only using the main chuck and upper tool spindle in a program we will also program a dummy operation for the second channel. In most cases the dummy operation would be something like a turret park. Then in the sync manager you have to sync every operation from channel one to that turret park in channel two. We have been working with Mastercam and DMG for almost two years and there are still quite a bit of work arounds to get the CTX machines to play nicely with the Mastercam Mill/Turn module.

[rusty.ross]

9 minutes ago, scottm085 said:

We have two CTX Beta TC 4A's and they have been nothing short of a pain to program. Ours have Siemens controllers that read Gildemeister structure, so maybe not the same situation you are in. What I do know is that for ours to run the controller needs code in both channels, even if you are only using one channel. For instance, if we are only using the main chuck and upper tool spindle in a program we will also program a dummy operation for the second channel. In most cases the dummy operation would be something like a turret park. Then in the sync manager you have to sync every operation from channel one to that turret park in channel two. We have been working with Mastercam and DMG for almost two years and there are still quite a bit of work arounds to get the CTX machines to play nicely with the Mastercam Mill/Turn module.

yes our machines are very similar as we have Siemens as well. I am attaching the zip2go file here for others to look.

DG-C31-TSD-S_rev_A.MCAM-CONTENT

[scottm085]

Unforturnately, we are still stuck on 2023 still so I can't look at your file. If you can send a 23 file I could take a look and show you how I process parts to make them run on these machines.

[scottm085]

We also have an NTX. Toolpathing is essentially the same between the CTX and NTX, using the sync manager is where it becomes challenging. The CTX controller breaks each tool path up into its own sub program and using the "syncs" in the sync manager is what creates the sub program. I don't want to get too far into the weeds here but for the program to run there needs to be an equal amount of sub programs in each channel, even if you are not doing anything on the other channel there needs to be dummy operations. At the beginning of each sub there is info that updates the controller on the status of the machine, for example, it will read a variable at the start of each op and see that either the main chuck is empty, has an unmachined part, or has a finished part. It constantly updates the status of both channels so that if you had to stop and restart, you could do so at any part of the program without having to sift through and line up wait codes like you would on an NTX machine. 

[scottm085]

Here is an example of syncing a simple jaw turning program. Notice that all the operations have syncs.

[Aaron Eberhard]

43 minutes ago, scottm085 said:

Here is an example of syncing a simple jaw turning program. Notice that all the operations have syncs.

Yep.  

 

There was a few setup issues on your part (Machine Properties > Job Setup).   I added a spindle toolpath for you and added the syncs.   

You can download my updated file here: DG-C31-TSD-S_rev_A - With Sub.zip

One thing to note is that each of those Syncs need to have a comment, or it'll give you an error on posting:

[scottm085]

Regarding the comments, it was taught to me by a DMG tech, that for the paths that work on the main spindle the comment needs to be "SP4" and for the sub spindle "SP3". For most situations the syncs have to be opposite from one another. In the screenshot i showed the comment for sync 1 on the upper channel is SP4 and the comment for sync 1 on the lower channel is SP3. 

[Aaron Eberhard]

13 minutes ago, scottm085 said:

Regarding the comments, it was taught to me by a DMG tech, that for the paths that work on the main spindle the comment needs to be "SP4" and for the sub spindle "SP3". For most situations the syncs have to be opposite from one another. In the screenshot i showed the comment for sync 1 on the upper channel is SP4 and the comment for sync 1 on the lower channel is SP3. 

Thanks for the additional info!   

 

Again, I'm not a DMG pilot...  I just helped a customer out with the Mastercam side, then handed it off, luckily I know they're quirky machines, especially with that weird canned language.

[Chris In-House Solutions]

The Mill-Turn post uses the structured code which is a bit to rap your head around.

When you upload the code on the machine the machine should have individual files for each operation/sub program.  I'm probably getting the terminology wrong here.  Its been a while since I've programmed one of these machines.  

7 hours ago, rusty.ross said:

For starters, the output has everything in one file, including the subs which coming from another siemens control I know they should be separated, right??

The last time I was onsite with this machine (beginning of 2020) the DMG tech gave the reasoning for the sub programs on the control being their own file and it made sense at the time.  I cant remember exactly what he said though so I apologize. 

This is a really neat machine I think you will like it once you figure out how it runs but that learning curve is steep compared with other machines.  There are not many people who have this machine so its tough to get information about how other people are running it.  

I'm pretty sure it accepts non structured (ISO) code as well but the techs prefer the structure code so its best to stick with what they prefer.  

[Greg Williams]

I have played with a few of these, are you using the DMG structure or running the MPF file?

[scottm085]

Quote

14 hours ago, Chris In-House Solutions said:

I'm pretty sure it accepts non structured (ISO) code as well but the techs prefer the structure code so its best to stick with what they prefer.

 

These machines do support ISO code. They should have also come with template files for your machine environment. You are supposed to use specific post templates for different machining strategies, pretty much like choosing the setup type in the "Job Setup" area for mill/turn. What I was told is that you need a separate template to run standard ISO code. We have not been able to get our hands on this template yet. I believe the template files are originated from DMG and they submit them to a reseller and then to the end user. As of right now there is not of surplus of knowledge in the US about these machines and/or post support for them. Everything I know has basically come from reading poorly translated documentation files and trial and error. 

[gcode]

4 minutes ago, scottm085 said:

As of right now there is not of surplus of knowledge in the US about these machines and/or post support for them. Everything I know has basically come from reading poorly translated documentation files and trial and error. 

That certainly doesn't sound like "turnkey" to me.

I wonder what they use to program these machines in Europe?

or are they so new all the CAM companies are struggling?

[scottm085]

From what I have heard, most of them use Partmaker. The software is not that great but it turns out pretty solid code. We have looked into other software solutions here as well, I don't think anyone has it totally figured out yet, we have seen a couple of demos from two of the bigger CAM companies and they looked pretty solid. We are not ready to jump ship yet, but are definitely hoping that Mastercam makes some strides to accommodate these machines in the near future.

[gcode]

I've never tried MT

We don't have any machines that MT supports.

We have a Mori Seiki NT6600 (that is now serviced by DMG) 

and an Okuma VTM-1200 YB. 

MT supports both the controls, but not those particular machines.

I asked and even offered to supply models but CNC was not interested in developing MT for either of them.

From what I'm hearing, that may have been for the best.

We drive both of these machines with Postability posts and get 99% post and go code.

Of course, the 2nd spindle and dual channel programs add a whole new level of complexity.

 

 

 

[Newbeeee™]

On 4/2/2024 at 3:12 PM, rusty.ross said:

Just a quick question that maybe one of you guys might be able to help me with. My co-worker and I are banging our heads trying to figure out what this machine is supposed to be doing. We bought a "turnkey" Mill turn software from Mastercam that hasn't worked since day 1. We have the code that Mastercam outputs but that is where we have hit a wall. Both Mastercam and DMG Mori have no idea what's going on, nor have they been at the machine to see it for themselves. We are at our wits end!
 

Every day goes by, is a day too long. Both DMG and your reseller need holding to account....

[#Rekd™]

Didn't  Bob W have issues with DMG and MillTurn dating back a few years or more?

[scottm085]

One of the last interactions with our reseller they had informed us that going forward they would not be offering this machine environment for mill/turn until the post and syncing issues were resolved (doesn't really help us). I don't know if they did or didn't but we feel left on an island a bit... We have had our machines for over two years and have yet to see any progress being made. From what I have heard the single stream CTX machines are fine with Mastercam Mill/Turn, the multi-channel machines are the real struggle since that is where the structured programming really takes effect.

[Aaron Eberhard]

18 minutes ago, scottm085 said:

One of the last interactions with our reseller they had informed us that going forward they would not be offering this machine environment for mill/turn until the post and syncing issues were resolved (doesn't really help us). I don't know if they did or didn't but we feel left on an island a bit... We have had our machines for over two years and have yet to see any progress being made. From what I have heard the single stream CTX machines are fine with Mastercam Mill/Turn, the multi-channel machines are the real struggle since that is where the structured programming really takes effect.

I would recommend calling into the Mastercam post department if you haven't recently.   I know that there was some work done by the German resellers in collaboration with DMG/Mori on these (I saw it on LinkedIn), so they might be able to give you some updated information?

[Newbeeee™]

1 hour ago, scottm085 said:

One of the last interactions with our reseller they had informed us that going forward they would not be offering this machine environment for mill/turn until the post and syncing issues were resolved (doesn't really help us). I don't know if they did or didn't but we feel left on an island a bit... We have had our machines for over two years and have yet to see any progress being made. From what I have heard the single stream CTX machines are fine with Mastercam Mill/Turn, the multi-channel machines are the real struggle since that is where the structured programming really takes effect.

I'm afraid at over 2 years....it's so long ago....it'll be seen as "not a problem".

As Aaron said - see if you can get direct contact into HQ and see what's the score. The problem with these situations, is machines are often more expensive than homes....but don't get treated accordingly. The old saying of he who shouts loudest, is very true, when you need a response  

2 hours ago, #Rekd™ said:

Didn't  Bob W have issues with DMG and MillTurn dating back a few years or more?

Damn Machine's Garbage....was by memory....

 

[scottm085]

We have had meetings with our reseller, post builders from CNC Software, and the guy from DMG who wrote the code for the CTX module/post from Germany. I think everyone agreed that they had some work to do! All of us were in a meeting together, which was nice, but unfortunately not that productive. At this point we're just dealing with the work arounds which is still a headache. It wouldn't be so bad if we were a high quantity production shop, but we are a high mix low quantity job shop which forces us to constantly be changing over setups and running new code on these machines. 

[Kalibre]

The machine support from DMG is pretty top notch, they moved some mountains when my old shop was getting through the commissioning of our CTX.

App support was decent, really good with anything controller related, absolute pants with CAM/post things.

Overall, I really liked that machine.

The only post solution IHS was willing/able to offer was an M/T environment that would post bare bones ISO. No Cycles (rough turning, threading, etc.), just good old line by line, "re-post if you need to change something at the machine".

I ended up just adding a ton of modifications to MPLMASTER and made a CHOOK to generate the MPF and SPF files after being told by the post department that they couldn't do it.

Hopefully there's better options available (doesn't sound like it from your post), but you guys should be all over them if the provided solution isn't coming close to expectation, it certainly wasn't provided cost free.