Z Zero to table??

[wayne_walker]

I normally Z zero to the top of the material.

I am cutting .375 ABS that measures .389 which is quite common. (this thickness can vary in the same sheet this much) However on this job I need to cut a recess area, so that the remaining material is .318 thick.



Using Part Wizard, I set material to Z from the bed, Z'ed to table, and called for the finish depth of .318. I cut a sample and it cut so the remaining material was .72 +/-. Thinking I set it wrong I deleted the tool path and re-did it. Same results. Now I think I am suppose to do the math first and then set the finish depth at .57 to get a remainder of .318, so I tried that with the same results.

I have tried this several times, several ways and can not seem to get it to work. I think I a doing it like the book says but I can not get the results I need.

TIA

Wayne

Using SB 3.4.27
PR upgraded to PRT
PC router
Part Wizard 2

[jerry_stanek]

What did you set as the thickness of your material? If you set the material .375 and cut to .57 deep that would leave .318 over the entire surface

[wayne_walker]

Jerry,

I set it at .375.

AND I set the cut depth to .57 and it left a thickness of .57. I restarted the program and had the same results.

It ask for FINISHED depth so I would think it should be .318!!?

Wayne

[tmerrill]

Wayne,

Not sure about Part Wizard, but with Partworks this is how I normally do what you are talking about. Takes an extra step but the results are accurate.

In PartWorks, set your material thickness for a little over what you would see as a maximum. In this case I would set it for 0.4". Then set your Z-zero from the top of the material and calculate your cut depth down to what you need left.

At your machine, Z-zero to the bed then move your Z to 0.4" and reset Z to zero (ZZ).

If you do a lot of similar cuts with the same material, you could easily create a custom file to do the set up at the machine.

First pass may be mostly air cut but there are ways to get around that.

Tim

[wayne_walker]

Tim,

It took me a minute to get it but I am sure it will work. I will give it a shot in the morning.

Thanks Tim and Jerry

Wayne

[wayne_walker]

Tim,

I tried your process and could not get it to work.
It brought up a message saying " could not continue, the finished height must be lower than the starting height". (Which it was!!!)

To confirm here is what I did...
In PartWizard
A.) Set to measure to the top of the TABLE
B.) Set the material thickness as .400
C.) Determined I need to cut out .078 of (air) and material to leave .318
D.) Set the finished depth to .318
E.) Hit calculate now... and the message poped up.

After this can up I...
A.) Set to measure to the top of MATERIAL
B.) Set the material thickness as .400
C.) Determined I need to cut out .078 of (air) and material to leave .318
D.) Set the finished depth to .318
E.) Hit calculate now... and the message poped up.

I then tried it both ways with the finish depth of .078 and got the same message.

Did I miss something in the translation or is PartWorks just that much differant?

Any help is appreciated.

Wayne

[tmerrill]

Wayne,

PartWorks is light years ahead of PartWizard and in the newer versions it works correct without doing the trick I described.

But back to PartWizard. You are trying to fool the software into thinking your block of material is 0.4" thick AND you are using the top of the material to set your Z-zero. I think this may be what you missed. Since you can't Z-zero to the top, because of the thickness variations, you "fool" the program by zeroing to the table, raising the Z to 0.4" and then setting Z-zero to 0.0 using the ZZ command. So you need to set up your toolpath to work from a Z-zero from the top of the material.

In other words, in PartWizard you would do everything the same way as if your material was 0.4" thick, you wanted to set Z-zero to the material top, and you wanted to cut down 0.072". But when you go to your ShopBot, don't Z-zero to the top of the material! Instead, Z-zero to the bed, raise it up 0.4" and then reset Z to zero.

If this doesn't work, forgive me. I haven't used PartWizard for ~4 years since Vectric started selling their products. I don't even have PartWizard on my computer anymore.

Tim

[thewoodcrafter]

Like Tim said "PartWorks is light years ahead of PartWizard"

It you possibly can, consider buying V-Carve Pro or PartWorks.

WAY better program and much easier to use. I never could get the hang of ParWizard. Very clunky program.

[tparr]

Has anyone figured out a way to import PartWizard files into PartWorks or Aspire?

[tmerrill]

Thomas,

Without having PartWizard anymore, I can only guess that you can use the Window's clipboard to copy and paste vectors from PartWizard to PartWorks/VCP or Aspire. This won't import toolpaths but with the improvements in PartWorks/VCP/Aspire, I would want to recalculate the toolpaths anyways.

Other than this, PartWorks/VCP/Aspire will import .dxf, .dwg, .eps, .ai and .pdf (vector) directly. If PartWizard will export any of these then that may be a possibility.

Perhaps someone who has PartWizard and one of the Vectric programs will have more to contribute.

Tim

[Gary Campbell]

Thomas & Tim...
It has been some time, as we are using VCPro, but if I remember previous posts, a PartWizard file can be read by an ArtCam or Insignia user. ArtCAM or Insignia can convert the vectors to DXF or EPS and those vectors can be imported into the Vectric products.
Gary

[oddcoach]

You could cheat
Zero the bit to the table then move z to .318 and zero z there then use 0 as your depth of cut
John

[Gary Campbell]

Wayne...
Most of us that cut cabinets with dados do this on a regular basis. Sheets vary in thickness by as much as .040 both from sheet to sheet and even within the same sheet.

To ensure consistant dado tenon thickness' we need to assign an "average" depth and then set a cutting depth that results in properly dimensioned tenons. Here are the steps, as I feel you missed one above:

(Using your exact numbers)

Zero bit to spoilboard
MZ to .389
ZZ to set zero at .389 above bed
Toolpath with "zero to top of material" settings
Set finish depth (or cut depth) to .71 (.389 - .318)
Do not select zero to bed toolpath parameters!
Gary

[zeykr]

Think Gary means .071 instead of .71

[Gary Campbell]

Ken...
YES I DO!!!!
GC

[curtiss]

RE: Ken... YES I DO!!!! GC

Those darn decimal points on the Z axis can really make a mess sometimes...

x & y not so much....