contour

[Tom]

Hello folk,

I'm working on a simple 2D contour ( a circle ) In this program, I need to program such that the cutter starts at the bottom ( final depth )

of the contour first and then cuts contour several paths upward ( rough step)

I'm wondering if there is a way to do that without defining mutiple circles and operations

I'm using V8.1.1

your help is appreciated

[cadcam]

Tom I would have to say no, unless it was a surface contour then you can choose from the bottom up.

May i ask why you want to do this?

Thanks J

[Glenn Bouman]

You could do the contour at the final depth and then use Toolpath, Transform and translate the toolpath in a z + direction with a number of copies

[P_Scott]

Tom,

I tend to agree with Jay. I tried to repeat what you wanted to accomplish with the Circle Toolpaths. Circle mill is similar to a Contour but always starts from the top. Thread mill has a Helical contour and will start from the bottom and go to the top but has no roughing method. I tried to mirror or rotate the circle mill toolpath to see if I could get it to start at the bottom and work up, but that wasn't working either.

Actually, you may be able to create a Circle mill toolpath, Transform rotate it from the Front Cplane and then post it out. You would then have to edit the NC code file so it wouldn't attempt to rapid and feed the tool from the backside of your part. Hope this gives you some ideas.

[P_Scott]

Glen,

I wish I had thought of that. My ideas wee just too complicated.

[Keith Graydon]

Tom, It's not too hard.

I got a .5 mill interpolating a 3.0 bore from the bottom up in 4 steps of .25 increments. Edit one line of posted code and your set.

quote:

---

TA,1

%

N1O0000(PART)

N2G0G17G40G49G80G90H0E1Z0

N3T20M6(.499 DIA END MILL DIA. - .499)

N4G0G90S3000M3E1X1.2505Y0.

N5H20Z.25

N6A-0

N7G1Z-1.F11.

N8G3X0.Y1.2505I-1.2505F24.

N9X-1.2505Y0.J-1.2505

N10X0.Y-1.2505I1.2505

N11X1.2505Y0.J1.2505

N12G0Z.25

-------DELETE THIS LINE--------

N13Z-.75

N14G3X0.Y1.2505I-1.2505

N15X-1.2505Y0.J-1.2505

N16X0.Y-1.2505I1.2505

N17X1.2505Y0.J1.2505

N18G0Z-.5

N19G3X0.Y1.2505I-1.2505

N20X-1.2505Y0.J-1.2505

N21X0.Y-1.2505I1.2505

N22X1.2505Y0.J1.2505

N23G0Z-.25

N24G3X0.Y1.2505I-1.2505

N25X-1.2505Y0.J-1.2505

N26X0.Y-1.2505I1.2505

N27X1.2505Y0.J1.2505

N28M5

-------ADD A RETRACT HERE FOR SAFTEY--------

N29G91G0H0Z0.

N30E0X0Y0

N31M30

%

%

---

Program the first cut to the depth wanted.--Z-1.

do consecutive COPY AFTER'S in the Ops Manager. Then set the Z depth in each of the OPs. THEN.......

TOOL PARAMETERS TAB /Change NCI button/ ensure "force toolchange" is UNCHEKED.

CONTOURS PARAMETER TAB on each OP.

uncheck Clearance

uncheck retract

set FEED PLANE = to depth of cut.

 

HTH

KLG

[cadcam]

I would say that Glenn is about as close as you can get to what he asked but still has more then one op.

But i do say there are many ways to skin a cat.

[Keith Graydon]

Glen's solution is good. However, the tool does retract from the work between steps. Mine solution forces the tool to stay in the cut as a normal "top down" contour. Are we being graded on this?

 

KLG

[cadcam]

quote:

---

Are we being graded on this?

---

Keith Graydon, if we were you would get an "A" for one of the great ways to skin this cat.

[Tom]

folks,

At first, I would like to thank you very much for all the replies and solutions to my question

In reply to you folks question earlier. I will describe a little more detail what I'm trying

to do . I'm working on a program to cut a body of a mutiple pin electrical connector.

In this program, after drilling more than 100 deep holes, I need to put an undercut near bottom of each drilled holes

To cut these undercuts. We modify a carbide endmill to a very small diameter keyseat cutter.

The width of the cutter is much smaller than the undercut area that need to be cut to reduce the pushing force to the endmill

Therefore. It needs to travel several paths and technicaly, We want it starts to cut in the middle of the area. Cuts a

few circles upward and downward

Because, This whole operation will then be transformed to another 108 locations ( 108 pin connector )

so I'm afraid any transformed toolpath in the source operation would not be working in this particular case

[Travis_Buchanan]

108 Locations? Sounds to me like a great place to use an incremental sub-routine.

--- MAIN PROG BODY ---

G00G90X-1.Y-1.

M98P0005

G00G90X-2,Y-1.

M98P0005

.

.

.

------------------

O0005( SUB CYCLE )

G01G90Z-START DEPTH

G91

G01

G03

.

.

.

G00G90Z1.

M99

[gstephens]

I would just model the toolpath. Offset the geometry to get tool center, create your lead in/out moves, copy it 4 times, create the vertical transitions, and do 3-d contour of it (chain-partial with wait turned on will be easiest).