I was wondering how do u guys make an arc on the Hurco milling machine going from x.5 and z.5 with .25R then x.5 and zo again with .25R? I was making those "thumb screws" using a ball endmill for the sides and had to do that top arc by laying down the milled thumb side then do the arc but I wanted to do it all in one shot without too many ops.
I called Hurco about that and they said something about "3d machining" which we don't have installed. I know I can do it in any angle but an arc?

What hurco is this on?

VM2....only thing installed on it is the DXF format.

BMC 30 that's what we got, I was wrong with the other posting. Sorry.

send me a pic or drawing of what you are trying to do and I will help if I can. Use to be the Senior App. for Hurco. gsilberberg@progressive-plastics.net

Let's see if I can "write" a picture to you.
Stock is 3/4th diameter and one inch tall on one end with 7/16 - 18 thread and two inches long on the other end.
Top of the stock becomes 3/16 wide with each sides having 5/8th ball endmilled flares out to the 3/4th diameter. Then the top having an arc going across along with the 3/16 wide by 3/4th diameter, arc or rad being about 1/2. (Note all that is for looks and feel on your fingers as in those thumbscrews)

Fax me a hand sketch. 765-552-7773 to George

Could you program the whole part with the G&M side of the controller? Then you could use G17, G18, or G19 to change the plane.

You can but in the past Hurco was backwards on cw and ccw when you switched planes. I just cut a cavity with our hurco and programed m and g and went with small step overs and made a nice looking round that the axis runs parallel to the parting line.

Fax me a hand sketch. 765-552-7773 to George

Sent from work as I didn't have a Fax.

I got the fax. Hurco's 3d would work for this. But you could also do it with mastercam or bob cad at a greatly reduce price from what Hurco wants for their 3d. I would use the NC side and do a program with Mastercam or bobcad. Either would do it and Bobcads prices are good.

open a milling block - - lines and arcs - - 3d arc. arc can be struck from any point to any point. fill in the blanks. if you need multiple arcs along a line or rotated about a point, use loop linear or loop rotate pattern. poor man's conversational 3d. ron

I'm having do do somethig similar, I have to go from x0z0 to x150z5r24000 and x400z0r24000, but I don't know those parameters for a 3d line, where do I enter the arc? I do many programs like this in G code usign diferent controls like MAZATROL, FANUC, ACRAMATIC, but this time I want to do in the conversational editor...

julio_qyn
Is this type of code of any use?
This is the profile path from X0 Y0 Z0 to X150 Y0 Z5 with radius of 24000 and stepover of 5.
Would need to know what dia. ballnose cutter to be used to generate tool path.
Advise if interested.

G01 X0 Y0 Z0
G01 X4.9977 Y0 Z0.1515
G01 X9.9954 Y0 Z0.304
G01 X14.993 Y0 Z0.4575
G01 X19.9906 Y0 Z0.6121
G01 X24.9882 Y0 Z0.7678
G01 X29.9858 Y0 Z0.9244
G01 X34.9833 Y0 Z1.0821
G01 X39.9807 Y0 Z1.2409
G01 X44.9782 Y0 Z1.4007
G01 X49.9756 Y0 Z1.5615
G01 X54.973 Y0 Z1.7234
G01 X59.9703 Y0 Z1.8863
G01 X64.9676 Y0 Z2.0503
G01 X69.9649 Y0 Z2.2153
G01 X74.9622 Y0 Z2.3814
G01 X79.9594 Y0 Z2.5484
G01 X84.9565 Y0 Z2.7166
G01 X89.9537 Y0 Z2.8857
G01 X94.9508 Y0 Z3.0559
G01 X99.9478 Y0 Z3.2272
G01 X104.9449 Y0 Z3.3995
G01 X109.9419 Y0 Z3.5728
G01 X114.9388 Y0 Z3.7472
G01 X119.9357 Y0 Z3.9226
G01 X124.9326 Y0 Z4.0991
G01 X129.9295 Y0 Z4.2766
G01 X134.9263 Y0 Z4.4551
G01 X139.9231 Y0 Z4.6347
G01 X144.9198 Y0 Z4.8153
G01 X149.9165 Y0 Z4.997
G01 X150 Y0 Z5

this is g code, i can do it, but i want to do in conversational mode, 3D lines...

Suggest you draw on the XY Plane and change to ZX, YZ or Incline Plane.

I will check on the control wich options do I have.... tks...

julio,

All you need to do is Start a lines & arc block. Position your tool where the arc will start in X,Y & Z. Leave tool position "ON" (cutcom off). Press "advance, Next or right arrow. Select 3-D arc. (You do not need any software options.) Enter the point where the arc will end ( X, Y & Z point). On the right hand side of the screen enter any point which the arc will pass through. That's all there is to it.

GL

ML97

..... On the right hand side of the screen enter any point which the arc will pass through....

Does this point need to be calculated from the drawing?

Yes. The Hurco "auto-calc" feature does not calculate the ending point using a 3-D arc. If you have purchased the optional 3-d "mold package" it would then calculate the ending point for you. It's a nice package but if you just use 3-D occasionally maybe an overkill as if memory serves it was around $3K USD.

ML97

BTW
I still have one new option disk in my archives.
Let me know if you have any interest.

It was the intermediate point I was referring to.
I would assume the start and end points would be shown on the drawing.

Maybe stated a different way... "An arc which passes through any three points". Yes any point which lies along the path of the arc would work. The start or end point would not define an unambiguous arc. I know. Just pick a point which is easy to define.

ML97

now that make sense to me, I will try this when the jig is ready for machining

thanks,

julio

well, I had enough problems with hurco for that job, i spent 1 day and nothing... then I moved the job to another machine (DAH-LIH with FANUC) and in 5 hours i had my samples, perfect, rsrsrsr... the problem with hurco is, if I need to ajust something I have to go to the computer and change, then I have the new center for the arc, this is out of question, the job is 2 jigs with blades, I have to machine the top (2 arcs) and then in a second jig mill the land (2 more arcs) inclinated 30 deg... the material is not perfect flat, so, when is more warped I have to increase or decrease de hights... but I'm running another job on the machine, simple blades, 15 deg chuck no arcs, just 1 line... there is something good on that machine, the amount of coolant delivered....

I understand. Unless you have the optional 3-D mold software you have to calculate the points & center manually. The Option runs $3k if memory serves. I might still have one somewhere if you're interested.

ML

maybe sometime I will try small tests.. but for now I will run this kind of job in fanuc or mazak controls, the nc is more eficient for fast programs and ajusts... we have 4 disks, one is the 3d mold, I don't remember the last 3

When you're ready let us know. The 3D option is pretty easy and very powerful. It's not for all 3D stuff but can do some very amazing feats.

ML

ok, soon as I start another trickie job on that machine I came back...

3D Arc will work fine for this!! Ron Meyer is absolutely correct.