Drilling Problem in Quickcam 2D

[boots]

After setting up a multible hole pattern to drill, using Quickcam 2D, and runnng it thru the Cam Wizard and post process. When I run the .fnc file, the Micromill 2000 won't withdraw the drill everytime. It trys to drag it sideways thru the material to the next hole and the machine doesn't hold Z zero. I set the offsets and then check the offsets using the MDI. After trying to run the program and stopping it before breaking the tool, using the feedrate override & the Red stop button on the screen, I rechecked the Z zero using the MDI and the cutter was a good 6mm lower into the material. After re-homing the machine, I checked the Z zero with the MDI and it was correct. On a different file with lines and text, "follow" machine plan was used and it worked just fine.
Any ideas on what to look at?
Thank you

[Denford Admin]

It certainly sounds like the machine is stalling in the Z axis.
If the cutter is lower than it should be, then it must be stalling as it retracts out of the holes.
What material are you drilling ?
What size and type of cutter are you using ?
Try lowering the feedrate settings.

[Steve]

I agree with admin.

The machine must be stalling as it starts to retract then is out of position.

I do not think the material will make any difference as the stall is happening on the retract.

I would make sure the Gib strips on the Z are correctly adjusted.

Oil the z leadscrew and put some grease on the slideways. (you should have been supplied with Kluber grease when you bought the machine)

Run the program without material to check it out and you will hear if you have a stall.

Reducing the feedrate will help as the axis motor has more torque at lower speeds.

[boots]

I used the “Drilling” Machine Plan to create the post process. Why would the Z axis stall using this program from Quickcam 2D, the feeds and speeds are set with the material selected?
I’ve tried lowering the federate in the program to 50mm/min, was at 100mm/min, same problem.
The machine works perfectly with programs that are from Millcam Designer and I laid out the same pattern in Quickcam 2D using the “Inside Offset” machining plan, ran thru the file just fine, machine held Z offset.
I’m using a piece of acrylic with an 1/8” ballnose cutter with a depth of 1mm. These were more like the dimples in dice I was trying to make, not deep/thru holes.
I had to go thru every tab and option to find the machine I was using before running the CAM Wizard, this should come up automatically very early in the program like the “Billet Dimensions” screen that pops up at the beginning or at the beginning of the CAM Wizard portion. Really had to look to find the correct machine to choose. And what are the meanings of these different file extentions, .mml, .dmm, .mof, ..ncf ????
There must be a “bug” in the Drilling Machine Plan option.

[Benny]

"I had to go thru every tab and option to find the machine I was using before running the CAM Wizard, this should come up automatically very early in the program"

We noticed that the "Select Machine" under Options Menu is no longer in the latest version of QC 2D, however it was in earlier versions. Possibly deleted in the source code by mistake???

[Denford Admin]

The latest version (1.3 on) does not use the same method of settings materials.

It has been changed to use the current settings in vr milling 5.

Here is the note from the v1.3 release:

4. Materials and tooling editing has been simplified, and will use VR Milling V5 tooling and materials, if it is installed

If V5 is not installed, then a generic material and tool file is used which you can change within QuickCAM, otherwise it finds the current files you are using within V5, and uses those settings.

V5 is the master, so if V5 is open - you will not be able to change anything in QuickCAM 2D. You are best changing the settings in V5 and then running QuickCAM as it reads the files when it loads.

[boots]

I have Quickcam 2D V1.4 loaded.
I went thru the program line by line in notepad and lowered the feedrate to 5(mm/min) in the drill cycle. The program ran perfect in VR Milling V2.31.
I tried the same program in VR Milling V5.13 and it lost the Z again and ran the mill sideways into the billet. The feed rate was very fast in the drill cycle not like the slow rate that VR 2.31 ran in the program.
I used a piece of acyrlic just to test.

[Denford Admin]

the only reasons I can think causing the different results will be to do with contouring (turbo mode) and the type of control / firmware revision.

let us know what these are all set to and whether the problem still occurs when not in turbo mode.

vrmilling v5 is faster at getting moves to the control, and may be pushing the limits of the micromill steppers

[boots]

I'm using a Micromill 2000 with a Denstep card (red LED display). The feedrates in VR 2.31 are as follows; Default 100 Max. X, Y, Z, 500 Min. 20 Steps 314.96 Max Contour 300 Max Contour Angle 30 Jog 400. They are the same in VR 5.13 except Max Contour is 400.
I ran the program without Turbo and it ran fine.
I tried it again with turbo and the Z stalls on the retract portion of the program, usually on the second drill cycle then keeps stalling on each retract cycle. The machine will then stall on the down stroke when the Z hits its physical limit after about 5 drill cycles.
I removed the cutter and deleted the M03 spindle command and I can hear the stepper motor stalling in the retract cycle.

[Denford Admin]

Looks like V5 is set to try and run the machine quicker in Turbo mode - what happens if you drop the max contour feed to 300 in V5 ?

[boots]

In VR v5 I set the Max Contour to 300 and Turbo On and the Z still stalls on the retract cycle.

[boots]

This Z stalling in the retract cycle only happens in the "Drilling" machine plan. When I run another program using the "Follow" machine plan for engraving graphics it runs fine using Turbo, no stalling in the Z.

[Denford Admin]

Does V5 look to still be faster at drilling ?

We have changed V5 parameters to talk to newer machines as the electronics changed (and got better)

Maybe you should stick with V2 on older machines, and use V5 for newer or upgraded ones that have the new control card (with better contouring control) and high voltage to the steppers.

Legacy machine support in V5 can't be guaranteed to work 100% because we don't have the older machines to test on - if you can downgrade the setttings in V5 even further to make this work then let us know and it could be changed in product.

[boots]

In the Drilling mode V5 in Turbo was much faster.
In the Follow mode there was very little difference between Turbo On and Off.
I'll try some lower feed rates in V5.

[boots]

I tried several lower Max feedrates and Max countour speeds, all the way down to 200 Max & 50 Max Contour. Still stalling the Z in Turbo mode. You can hear the Z stepper motor stalling on the retract, even at these lower feedrates. This time it got thru the first hole cycle then stalled on the retract of the 2nd hole. Before it always stalled in the first hole.

[Denford Admin]

it looks like you won't get v5 to run the old control card slow enough in turbo.
a drilling cycle would be ok in none turbo mode.
the comes down to the fact that v5 is setup to talk to the new control cards and firmware which have better acceleration control of the axes. v5 will buffer any moves to the control, and it will decide whether to slow down across a sharp direction change.
because v5 is talking to an old control card, it is still sending all buffered moves, but the control is not clever enough to slow down over a sharp direction change. its changing direction in Z as soon as it hits the bottom of the hole, without decelerating first.

[Steve]

In addition to this since 1995 we have fitted a different transformer in the back of these machines. This splits off the logic supply 24V from the motor supply and allows us to drive the motors harder.

Machines fitted as standard with the new transformer and distribution board will have better performance than older machines.