Help needed with a “Z” problem

[Donna Ashby]

I’m not having any Googling luck trying to fix my problem.

I received a request from my neighbors for a name sign to hang on the stall of a new horse. This will be the 3rd sign that I’ve done for them. I just copied and changed the horse’s name on an older file that had previously ran successfully.

Using Aspire 8.5 and a Camaster Stinger.

Aspire job dimensions were set for the new board thickness (~.1 inch thicker). Everything recalculated and tap files saved. The Aspire Preview looked correct, the images of a horse with a barbed wire border were inset like I had intended.

Camaster touch top calculations were right on, paper in between the work and the bit just catches. Tried zeroing it manually anyway.

Tried both the single tool post processor and ATC post processor. Even tried an edited pp from a few years back that had had a Y axis glitch.

When I run the first file that begins the rough out for the inset images, the bit doesn’t go down into the wood at all. It remains slightly above the work surface.

I’d be very grateful if someone could point me in the right direction. It’s been a couple of years and an Aspire upgrade since I last did a full project beyond checking, oiling and making sure the machines were functioning. Can the measure tool length process glitch things even though Z0 looks good?

Thanks for any help.


Sorry for the mixed up title, something to do with my ipad I imagine. Is there a way to edit the title?

[Grant Wilkinson]

Can you either post the .crv3d file or send me a pm with it attached? I'll take a look at it.

[David Buchhauser]

I’m not having any Googling luck trying to fix my problem.

I received a request from my neighbors for a name sign to hang on the stall of a new horse. This will be the 3rd sign that I’ve done for them. I just copied and changed the horse’s name on an older file that had previously ran successfully.

Using Aspire 8.5 and a Camaster Stinger.

Aspire job dimensions were set for the new board thickness (~.1 inch thicker). Everything recalculated and tap files saved. The Aspire Preview looked correct, the images of a horse with a barbed wire border were inset like I had intended.

Camaster touch top calculations were right on, paper in between the work and the bit just catches. Tried zeroing it manually anyway.

Tried both the single tool post processor and ATC post processor. Even tried an edited pp from a few years back that had had a Y axis glitch.

When I run the first file that begins the rough out for the inset images, the bit doesn’t go down into the wood at all. It remains slightly above the work surface.

I’d be very grateful if someone could point me in the right direction. It’s been a couple of years and an Aspire upgrade since I last did a full project beyond checking, oiling and making sure the machines were functioning. Can the measure tool length process glitch things even though Z0 looks good?

Thanks for any help.


Sorry for the mixed up title, something to do with my ipad I imagine. Is there a way to edit the title?

Please post your file (dxf, crv, etc.) and I will take a look at it and try to help you.
David

[David Buchhauser]

I’m not having any Googling luck trying to fix my problem.

Can the measure tool length process glitch things even though Z0 looks good?

Yes. It's very important to have your actual tool height set properly. Aspire doesn't know what your actual tool height is. Try lowering your cut (depth) in Aspire and run the program again to see if the cut depth in your wood part corresponds with the numerical change in the program.
David

[David Buchhauser]

I’m not having any Googling luck trying to fix my problem.

Can the measure tool length process glitch things even though Z0 looks good?

Yes. It's very important to have your actual tool height set properly. Aspire doesn't know what your actual tool height is. Try lowering your cut depth in Aspire and run the program again to see if the change in cut depth in your wood part corresponds with the numerical change in the program.
David

cut depth.jpg

[Kevin Jenness]

You may need to calibrate your tool height relative to the touch pad if you are using the ATC. I have FTC ("fast tool change" with manual bit change and automatic tool height check). With my machine after surfacing the table or screwing up the calibration somehow I have to bring a bit to the table, then run the calibrate tool routine to establish the offset between the table and touchpad. If you are using the single tool post processor you need to lower the bit to the table, zero the Z axis and go from there. If you have the material thickness and the cut depth set correctly in your toolpath the problem is probably in the tool height indexing relative to the table.

[Donna Ashby]

I've been looking at my tap files and I can see where z isn't going negative or negative enough in the tap files that have to do with modeling. The final cut out tap files using an end mill and the name carving tap file using a v bit all have z values that I would expect to see. So I must be doing something wrong with the image modeling. I'm going to paste an excerpt of the first tap file that is roughing out the images with a .25 BN. Notice in the tap file that z doesn't go negative. One of the things that has me baffled is that the tap file from the sign that I cloned looks the same. I'm not sure how to include a copy of the Aspire file, it's fairly large. I think I'll go down to my machine and test out the definition of insanity one more time, paying close attention to the order of setup and measuring of the tool length and material top.

[VECTRIC CNC OUTPUT FOR CAMASTER SINGLE TOOL ]
[MACHINES WITH WINCNC CONTROL ONLY]

[FILENAME: testing 3d roughing]
[01:07 PM, Tuesday August 11 2020]

[MATERIAL size: 15.000" x 8.000" x 0.827"]
[Z Zero Position: Material Surface]

G90 [ABSOLUTE MODE]

M5 [SPINDLE OFF]
G53 Z0 [LIFT Z TO TOP]

[Ball Nose (0.25 inch)]

S12000 [ SET SPINDLE SPEED RPM ]
M3 [SPINDLE ON]

G53 Z0 [LIFT Z TO TOP]

[TOOLPATH NAME: 3D Roughing 2]
F100 XY [SET FEEDRATE FOR X AND Y]
F30 Z [SET FEEDRATE FOR Z]
G0 X13.703962 Y2.879054
G0 Z2.000
G1 X13.703962 Y2.879054 Z0.029984
G1 X13.703962 Y2.857684 Z0.030000
G1 X13.678962 Y2.841191 Z0.030000
G1 X13.678962 Y2.878747 Z0.030000
G1 X13.675799 Y2.878708 Z0.030000
G1 X13.653962 Y2.872594 Z0.030000
G1 X13.653962 Y2.851157 Z0.029359
G1 X13.653962 Y2.824361 Z0.030000
G1 X13.628962 Y2.808511 Z0.030000
G1 X13.628962 Y2.829532 Z0.029258
G1 X13.628962 Y2.840043 Z0.028907
G1 X13.628962 Y2.861064 Z0.030000
G1 X13.628962 Y2.866319 Z0.030000
G1 X13.603962 Y2.860417 Z0.030000
G1 X13.603962 Y2.838350 Z0.029207
G1 X13.603962 Y2.827316 Z0.027974
G1 X13.603962 Y2.799732 Z0.029991
G1 X13.603962 Y2.794215 Z0.030000
G1 X13.584488 Y2.783879 Z0.030000
G1 X13.578962 Y2.778781 Z0.030000
G1 X13.578962 Y2.805853 Z0.029411
G1 X13.578962 Y2.816682 Z0.028096
G1 X13.578962 Y2.838340 Z0.029736
G1 X13.578962 Y2.854584 Z0.030000
G1 X13.553962 Y2.847400 Z0.030000
G1 X13.553962 Y2.825879 Z0.029171
G1 X13.553962 Y2.809739 Z0.026629
G1 X13.553962 Y2.777457 Z0.029853
G1 X13.553962 Y2.761317 Z0.029992
G1 X13.528962 Y2.749857 Z0.029982

[Kevin Jenness]

You have Z zero set to the material surface while the G code is sending the bit to positive Z values. The bit, naturally, is not contacting the workpiece. If your bit is indexed correctly to the table then perhaps, as you surmise, the problem lies in the placement of the model in the material.

I always use the table as z zero rather than the work surface.

You said that the toolpath preview looked correct. That suggests to me that the issue is with the tool height calibration rather than in the Aspire toolpath.

Have you tried posting your Aspire file on the Camheads or Vectric forums?

[Donna Ashby]

I contacted Vectric support and sent them the relevant files. Hopefully they can figure out what I'm doing wrong.

[Ronald Blue]

Have you had any success Donna? This is the type thing I have go wrong occasionally.

[Donna Ashby]

Yes, the lightbulb finally came on. It did have to do with the roughing toolpath .03 inch machine allowance. A good part of the inset barbed wire was shallow enough that the .03 allowance put the bit above the material top. The tap file still did all the maneuvering of the bit even though it was over the surface. So basically, I just had to wait for awhile before any cutting happened. If I would have looked closer at the preview I would have noticed that most of the movement of the bit was not actually cutting. I was mostly looking at the preview without the blue lines displayed. This was the third sign I had done for my neighbors but there was a break of several years between the first 2 and this one. I was much more immersed in the CNC and Aspire programming back then and apparently figured out what the issue was, but then I did a brain dump between then and now. Well, it did come back but it took a while...