That was GREAT - now lets try this!

[tlempicke]

O.K. guys you came up with a couple of good ways to answer my last question, here is the next one.
I am cutting a piece out of 1/2 inch plywood. I want to cut 1/4 inch down on the first pass and then 1/2 inch down to finish the part.
I selected .250 and .500 in the appropriate boxes of the profile page. When I selected the 1/4 inch end mill I set the step down to .250 inch.
when I generate a tool path it cuts .500 deep in one pass.
I can, of course, generate two separate tool paths and then save them in order (In fact I did this) but then the tool must return to the zero point between passes.
Is there a better way? If not what are the boxes that I am filling in really used for?

[billp]

Tom, I just used the same technique you mentioned to generate a profile and also I "machined along vector". In both cases I generated two passes of .25 each.I usually use this same method of "lying" to the program by telling it my bit can only stepdown a specific distance, and the program will automatically make the cut in two passes.
When you say you filled in both .250 AND .500 in the appropriate boxes , which boxes are you using? I only see one box for depth of cut.
Did you change your bit stepdown by editing it in the tool database?

[tlempicke]

Bill
As a test I opened a new model and drew a circle. I then went to Profile. Filled in the screen thusly

Outside
Start Depth .25
Finish depth .5
Safe Z .25
Profiling tool 1/4 inch end mill with stepdown of .25
Cut direction conventional
Name test

When I generated the toolpath I got this for the first few lines

MS,0.7,0.2
JZ,0.250000
J2,0.000000,0.000000
J3,1.444110,6.577582,0.250000
M3,1.444110,6.577582,-0.500000
M3,1.444110,6.574418,-0.500000
M3,1.445629,6.457510,-0.500000
M3,1.450084,6.341316,-0.500000
M3,1.457440,6.225875,-0.500000
M3,1.467661,6.111224,-0.500000

As you can see it is going to cut .500 deep.

What did I miss?

[billp]

Tom, I may be missing some of the nuances in PW, but I used a start depth of "0" since I am going by the rest of the Delcam line ( Artcam Pro, Insignia) and using the surface as my zero point.
I'll be heading in to the shop shortly and I'll try to cut the file I drew up as a test..More to follow..

[billp]

Tom, I just redrew the file, checked the code, and ran it. I got two passes, the first being -.25, and the second -.5
I drew a circle in the PW software and then followed the steps outlined above. I ran the file , even though the code looked good, because I remembered that there was some question about PW and how it set up certain files. This procedure worked fine for me...

[billp]

Tom, here are the first few lines of my file...
MS,2.0,1.0
JZ,0.000
J2,0.000,0.000
J3,0.875,6.002,0.000
M3,0.875,6.002,-0.250
M3,0.877,6.131,-0.250
M3,0.882,6.262,-0.250

[jkforney]

Tom
Bill is right. You need to start at 0 depth. You set the number of cuts by your step down in your bit library. Be careful though, because if you want to cut .5 and you put in .375 you will get two passes at .25 not one pass at .375 and one at .125. It appears that Part Wizard will make even passes. .375 step down will go into .5 depth 1.3333 times which Part Wizard rounds to 2 and gets .25.

In Insignia (Part Wizard's big brother) you can input a final pass.

John Forney

[tlempicke]

YESSSSS! I started with a zero depth and it worked just fine!
Thanks again guys!