Gcode + post processor problems

[ecs]

Hi Guys,

I have a few issues i'm trying to figure out.

1. Why when i load the gcode the picture in masso is tiny? You can barely see what its going to cut.
   
2. My post processor puts a "G28 U0. W0." at the end and the machine takes off and goes all the way back to the homing switches. What is U and W? I have a X and Z haha
   
3. I have constant surface speed turn on and set tp 2000 RPM maximum @ 50m/min which equals to a rough rpm around 1500. When i try this the spindle doesn't even start up when it runs the program. It barely turns 10 revolutions the whole facing and turning operation.
   
4. My spindle takes to long to start up. Is there a setting in the VFD or masso to speed up the start time?
   

Thanks,
Josh

 

[al]

explanation of u and w for reference point return see link

G28 Reference Point Return - CNC Lathe - Helman CNC

G28 reference point return G-code is used to approach the reference point via an intermediate position. The intermediate position can be specified absolute X, Z or relative U, W.

www.helmancnc.com

 

[westyone]

@ecs Masso is scaling the graphic to include that G28 U0 W0 move. Delete that and the graphic will resize and the Lathe won't go all the way back at the end of the program.

On F1 screen, under "Spindle" check the "Spin up" delay. I use 100 milsec

Other issues I'm still thinking about.

Cheers

 

[masso-support]

Hi Josh

I have constant surface speed turn on and set tp 2000 RPM maximum @ 50m/min which equals to a rough rpm around 1500. When i try this the spindle doesn't even start up when it runs the program. It barely turns 10 revolutions the whole facing and turning operation.

I had a look at your GCode and you have a CSS set to 50mm per minute not 50 meters per minute That is why it is running so slow, off by a factor of 1000.

S Value To set surface speed value. The units will be the current machine units in use.​

N21 G96 S50 M3

AL and Westyone have you covered for the rest

Hope this helps

Cheers

Peter

 

[ecs]

@al - Thanks for that. I have now change the post processor to remove it!

@westyone - Cheers mate. I was doing this is the masso wizard. I have mine set to 5000. What size electric motor do you have on your lathe? Mines 7.5HP and i think that's why i needs such a big delay. I'm not sure i will look into this some more.

@masso-support - Thanks Peter! This is definitely confusing. It shows m/min in fusion but i have change it back to the default at 200m/min. I have altered everything and will give it a go when i get back to work.

Thanks for everyone's help!!

Josh

 

[ecs]

Hi Guys,

So those suggestions fix all of those problems but now i have new ones.

• Surface speed was set to 200 m/min as default but i had to increase it to 3000 m/min to get the rpm to run at 1200 on a 10mm part. Is that correct?
  
• Why does the spindle speed goes past the maximum set for the job then come back down. The spindles all over the place and far from what it should actually be. Please see video. https://drive.google.com/file/d/11FzSjq_cQbccAK8l5-ZMU32oRKMxvcld/view?usp=sharing
  
• Why does the G97 starting the spindle again on line N43?
  

I noticed the G50 code isn't on the masso which is meant to cap the speed to what its set to. I think thats why this is happening but would like someone who actually knows about cncs to speak up.

Josh

 

[al]

basic rule of thumb- to convert cutting speed to rpm is (CS X 4) divided by dia. = RPM (3000X4)/10=12000/10=1200 . This looks good (if you input 200 you get 80 RPM)

looking at your program you are using both G96 then G97 at different places

1. G96 Turn on Constant Surface Speed (CSS)
   
   
2. G97 Turn off Constant Surface Speed (CSS)
   

watching the video I think your looking at the part where the G96 is active this changes RPM with the Dia ( X axis position ) to maintain a constant surface speed , where as the G97 locks the spindle to a fixed RPM regardless of the Dia.

Masso does not use the G50 to cap Rpm

Check the settings in your post processor , the output G code is calling both G96 and G97 at different times , like the facing cut uses G96 to maintain a constant surface speed to get a good finish , the thread cutting calls a G97 to fix the rpm to make sure the pitch comes out correct

also looking at the video and the g code you posted I think you have the M4 and M3 reversed , the view of your lathe in the video shows the tooling and the spindle rotation for a M3 but the program calls a M4 , Its hard to tell but a quick check is to put a standard right hand drill in the tailstock MDI a rpm and M3 and see if it will cut

hope this helps

 

[cncnutz]

Whole lathes are not my thing, you are correct about the G50 not being supported.

You can however limit the RPM using the G96 command using the D parameter. In the example below it will limit it to 1200 RPM

N21 G96 D1200 S3000 M4

instead of

N20 G50 S1200
N21 G96 S3000 M4

I modified the G96 by hand if you want to give it a try and see if it helps

Out of curiosity, what post processor are you using to output your GCode?

cheers

Peter

 

[evermech]

Hi Josh,

do you think you could set up a scenario facing a part maybe 4" od and several passes to complete face operations? Then post a short video of that, it will give us more time to see what's going on. It almost seems like the reaction time on the spindle is slower than what's needed to get the result your after but hard to tell.

i think Gcode should be

N20 S1200 M4 Spindle speed and direction
N21 G96 S3000 Css enable and value

also the suggested feed and rpm settings are on the back of the insert pack for each type of insert. I usually feed at around .006" to about .012" per rev. Css setting is usually between 175" to 350" depending on material. Depth of cut can be almost anything but I try to get a depth that the carbide will break the chips nicely because I hate stringy swarf. If I'm really roughing hard then I will set up a second tool to do a light finish cut to maintain accuracy. I think you can multiply any of this by 25.4 to convert to metric values.

Guy

 

[machinedude]

when you calculate cutting speeds on a lathe your work piece diameter is what determines the speed because that is what is spinning and the tool is fixed, on mills the the cutter diameter is what will effect how fast it should be spinning.

so constant surface speeds are going to change as the circumference of the diameter changes. so if your facing the spindle should get faster the closer to center you get and should be a steady increase on those operations and when turning the speed will increase every time you take a pass on your part but will only increase at the beginning of the cut when tool is first moved closer to center for that pass and maintain that speed until your next pass is started. once again the closer to center get the faster the spindle should be running.

i was not paying attention to what exactly was going on in the video but this is how it should be reacting.

 

[machinedude]

not a metric guy but a good starting point for turning is .012 per rev on roughing passes and .006 per rev on finish passes on your feed rates, you can fine tune from there.7.5 hp spindle will do some serious work but personally i would not beat up on the collet's those are more for precision .

 

[ecs]

@al - Thanks for the feedback. I do understand that with the CSS turned on the lathe speeds up and slows , the problem is the lathe speeds up past the CCS and then comes back to the CCS speed. But by the time the lathe reaches the proper CCS speed the facing tool path has ran and its half way through the next operation. Yes i changed the M3 to M4. I did check this a while back in another post but i can see i must have interpreted it the wrong way. I'll change the command back and swap over some wires. Thank you!

@cncnutz - Thanks peter thats some great advice. I'll change the code and see if this helps! There is currently no Masso lathe post processor so i'm using a fanuc lathe one and have been modifying it. It was suggested from another user.

@evermech - Yes i have to agree. I do believe half the problem is because it accelerates past the CCS speed needed. Then by the time it comes back is finished that operation. Thank you for the speed and feeds. I will lock further into this once i have the CCS working correctly.

@machinedude - Thank you also for the speeds and feeds and info. I dont plan on doing anything to heavy duty in the collets. I'm just making M8 and M10 studs.

Also another note is when the lathe heads towards the tool change and should be slowing down it actually speeds up again.
This line of code - G97 S1200 M4 is at the end of the first 2 operations and it makes the spindle take off again. I'm not sure what its there for when the operation has been done and moving onto the next.

I will create a new file tonight on a 4" part like evermech suggested and take a new video and show the results. Thanks again guys.

Cheers,
Josh

 

[ecs]

So i created a file with the 4" piece and here are the results. I did have to edit the gcode like peter said to kept the RPM at the correct level. I did my testing at 2000 RPM to create a bigger range.

Video is here - https://drive.google.com/file/d/11YuAKjC9Ao50miLVyqzsNGuHqWvCq6Xr/view?usp=sharing

The vfd is still powering when the lathe is on retract. A good 3 seconds and then stops when the facing starts again. Its like the vfd and masso are out of sync. It only starts to power up just over half way through the facing operation.

 

[evermech]

Hi @ecs

That helps a lot. I think the motor settings are too slow to get the results you want. Some experimenting with accel and decel will probably get you there. Especially decel as it can't react fast enough when rapiding back for next cut. You may have to look at the settings in the vfd also if you can't adjust it entirely with the Masso settings.

Guy

 

[westyone]

My lathe does the same thing, especially with a heavy chuck. Masso won't control this, it's a VFD issue. Your VFD needs to have DC braking activated. Some VFDs require the addition of braking resisters. Some come with them installed.

Cheers

 

[ecs]

@evermech - This is what i think is the problem or part of. I had a look on masso in the spindle setup and there's setting there i have tried but none made any changes unfortunately. Looking in my manual for my VFD and i did find some info there. But wanted to check if you think these are the setting i should be playing with. See Picture.

@westyone - My VFD doesn't have a braking resister built in but does show it optional. This will be my next resort if i can't get it to work with the settings.

Does anyone have experience in buying a braking resistor? I heard they cost as much as the inverter if you buy from the manufacturer. I have found the size needed from the delta manual and was going to search ebay. Any thoughts on this?

Thanks,
Josh

 

[westyone]

Without the Breaking Resistor you have only two options (that I know of and use).

1. Insert a line manually just after the G1 X0 move that says "G97 S100". This will get the VFD slowing down as the X axis is retracting for the next facing pass. Before your next facing pass feed line insert G96 S??? M3. You'll have to do that for each facing pass.
   
2. Insert a Dwell (G04) at the start of the second, third and so on pass to give the lathe time to spool down. Sucks but it's the poor mans solution.
   

Cheers

 

[ecs]

Quote from ECS on September 19, 2019, 1:30 am

@evermech - This is what i think is the problem or part of. I had a look on masso in the spindle setup and there's setting there i have tried but none made any changes unfortunately. Looking in my manual for my VFD and i did find some info there. But wanted to check if you think these are the setting i should be playing with. See Picture.

@westyone - My VFD doesn't have a braking resister built in but does show it optional. This will be my next resort if i can't get it to work with the settings.

Does anyone have experience in buying a braking resistor? I heard they cost as much as the inverter if you buy from the manufacturer. I have found the size needed from the delta manual and was going to search ebay. Any thoughts on this?

Thanks,
Josh

@breezy - Your a VFD expert what is your thought?

@westyone - Hopefully i can get it better with some settings. I have a found a couple of braking resistors so hopefully someone with some more experience can shed so light.

 

[evermech]

Yes those are the settings you can adjust to some degree. What are they set to now? @westyone is correct that you may need a braking resistor to dump the excess energy that your vfd may not be able to deal with. When deceling too aggressively the excess of energy builds up inside the vfd and causes the voltage to go high in the dc bus. If it goes over the limit set in the parameters the vfd will fault. But after having said that you should be able to push it by experimenting with the accel and decel times to make the spindle more responsive. If you go too far the vfd will let you know. You may have to adjust the settings in Masso in unison with the vfd so none of the settings contradict each other. Your collet chuck doesn't have near as much mass as other larger chucks so there should be some room for you to adjust this.

Guy

 

[ecs]

@evermech - YAY its working!! They were set to 10 seconds. I ran some test and i now have it down to 2 seconds. I had it on 1 second and it was fine but 1 time it did get an error so i uped it to 2 seconds.

Here's a video - https://drive.google.com/file/d/11qw0ZIdP_4DCdFw3WOwsWyjr8Azqtir8/view?usp=sharing

I still think the masso isn't correct when its stopping the spindle. The lathe is still powering 2 seconds more after the retact starts. You can see and hear this if you look closely in the video right at the end when i move over to the screen to show where the lathes upto. Which is giving the lathe less time to slow down. Why doesn't it stop after the cutting is done @masso-support?

I'm still going to purchase a resistor for it to help it slow down. Its a Delta VFD but delta dont make a resistor for this one but do give the specs for one to suit...... I have found this on aliexpress - https://www.aliexpress.com/item/33039737633.html?spm=a2g0o.cart.0.0.45c73c00lX8VLM&mp=1

The manual says i need a 1500w 69 ohm so was going to get the 1500w 50 ohm as this was the closest. Do you think this would be suitable?

Josh