[starmack2001]

I just purchased a 1998 BMC 3017 with the SSM control. I'm familiar with hurco conversational programming from running one 15++ years ago. I'm 65 and semi-retired from being self employed, but I still work for kicks and grins and to make extra money. Now, the one thing that I can't remember on programming the hurco is how to set the side cutting depth on an end mill. I'm programming a outside frame on a part (4140 steel) with approx .400 stock on each side . I want to take about .125 depth of cut on the xy axis. Hogging mill, I'm old school. Z depth and peck depth is no problem. I know it's in the parameters somewhere but I can't find which one. The only one that seems like it applies is in the milling parameters on pocket overlap %. Tried changing it and nothing happened. Can someone explain to me in plain english where I need to go for this setting. I know that I can change the tool diameter and achieve the same thing, but then I have to rerun the program each time I change the tool diameter.

[gcude]

Sorry I don't know that control, I'm on Ultamax II, but I'm glad to see another member of the Hurco community posting. Congratulations on your mill purchase.

[bhurts]

The ssm machine your using is a ultimax 3 if I'm not mistaken?

Ben

[starmack2001]

The SSM control is just a single screen instead of the double crt set up that is most common with hurco. I toggle between the input screen and the cad screen on one crt. The programming is ultimax, not the ultimax 2 or 3, but it's the same as the twin screen. Input keys, input screens are the same, best I can tell. Same hot key functions under tool setup, part setup, and part programming. Right now I'm running the machine with 2 tools doing the same operation, but one tool's diameter is set over size to make it a roughting cut. The second tool is "on diameter" to do a second rought cut and leave stock for the finish mill. I should be able to this by multiple cuts with one tool and setting the depth of cut, but I can't find the parameter to make that setting. I'm running lines/arc instead of frame because I have a couple of 1" bevels to cut on one end of the part and I can't do that in the frame program. 95% of the parts that I make can be done on the conversational control, including ball sockets using the 3d mode. That's why I bought the hurco. I also have a HAAS that I program offline using featurecam.

[bhurts]

I am now unsure what is what. I have a bmc30ssm that is a 2 screen ultimax 3 from 97. I thought the ssm was because it uses dc brush servos instead of ac brushless.

Ben

[bhurts]

Now I am even more confused. From Looking online it seems ssm probably is for single screen but mine is definitely dual screen ultimax 3. I have the original purchase invoices and it came from the showroom brand new that way. I have all the manuels for it as well.( conversational programming, g-code programming, maintenance, and full schematics Manuel.)

Ben

[Rich Carlstedt]

His control looks like this

30"X, 18"Y, 24"Z, 1998 HURCO BMC-3017/SSM, 520 Machinery Sales, LLC Used Equipment Network

I have never used this one
Rich

[Rich Carlstedt]

Let me try this

If I read you right you want to use a roughing endmill to rough out a FRAME ( Mill > FRAME ).
Hurco automatically uses "Cutter Offset" based on the tool diameter to determine tool location when doing a FRAME, That is the tool diameter determines cutter path for INSIDE and OUTSIDE frames.
Now, I f you enter a FINISHING TOOL number, The program will offset the roughing Cutter to the amount you desire.
That offset is found under MILLING PARAMETERS , under the PARAMETER Settings.
In that section it will ask how much X and Y you want offset for roughing.
As long as you do rough and Finish in the same block, it is used
If you write separate Blocks , the cuttters will not use the roughing offset and will machine to your dimensions.

It sounds like you were trying to adjust the "Overlap for pocket or frame milling"
This is not what you are looking for. That overlap is how much the cutter goes past the starting point so no cusp (uncut material) exists at the point of start and stop on a frame.
POCKET OVERLAP is how much ( in percent) the cutter path overlaps the previous cutter path .. so a 50 % setting means a one inch diameter cutter will only see 1/2" of material on each of it's next passes..nothing to do with Depth Of Cut.
This is not the same as the cutter roughing/finishing "offset" you want IHMO
That is roughing settings under parameters

Maybe this will help you
Home - MANUALS
Go down to MILLING A FRAME

Rich
holler if you have a question or I am still not picking up on your concern

[starmack2001]

I just found out today that what I want to do supposedly cannot be done on a hurco except in the nc mode. Not programmable in the conversational mode. I'm trying to profile the outside perimeter of a 15.3 X 9.3" block of steel. I need to remove about .300" from each side. My plan was to take about .100 deep by side milling X .500 depth of cut (Z) and make multiple passes around the part until I had removed the .300 from each side. It would require 3 passes around the profile of the block. I do this routinely on my haas vf1, but I program it in featurecam and download it to the machine. I have been told that this can't be done in the conversational mode of hurco programming. I was hoping someone with more experience on the hurco could tell me how to program it in conversational mode.

Ben-- the ultimax 3 is an upgraded version of the older version ultimax that is in my machine. I don't know what the difference is as far as capability of programming. The first hurco that I ran was in 1990 and it was just the "ultimax" program. It was a km3p knee mill. It also had the dual screen setup, as was common with most hurcos back then. I don't know about the servo setups from then till now. Nice thing about the hurcos BMC series is the box ways versus the guide ways that haas and others use. The box way is much stronger than the linear guideways, allowing for heavier material weights, but not as fast. Linear guideways have weight limitations on them. Linear guideways were developed for faster speed/feed combinations, but lighter cuts.

[starmack2001]

Rich, thanks for your help. The settings that you list are not showing on the 1998 Ultimax package. You've got the general idea of what I'm trying to do, but it appears that the older version of ultimax does not have the capability to do what I'm after. I'm rying to do multiple roughing cuts on the outside of the frame in one data block and I can't find a way to do it. So, I just programmed multiple data blocks (line/segment) using copy block and changed the diameter of the tool to compensate. It's crude, but it's working. Then I copied the same data block for the finish mill. Crude but effective. I tried setting the pocket overlap % to different values and it didn't seem to affect what I was doing. Maybe I just didn't do it right. Don't know. So I switched to line / segment programming and it appears to do what I'm after.

[Rich Carlstedt]

I just remembered and thought you may be looking at milling a CLOSED CONTOUR , where the POCKET LEFT (etc) mentions a " MAX OFFSET"

This is where the cutter will make two passes around the frame ( or inside) to remove excess material .
Now this setting , with a 1/2" cuttter will allow you to remove upto 1" of material around a frame.
The MAX OFFSET would have .749 as the number to use . That means the 1/2 cuttter CENTERLINE is .749 from the profile on the first path to remove .999 material and the second pass would be up to the profile .
That formula states one diameter plus One radius = MAX OFFSET ( so 1/2" + 1/4" = 3/4" )

Rich
The newer controls may use different terms, so I hope I haven't confused the issue
Also try this URL and click on Winmax Mill Manual for help
Home - MANUALS

[Rich Carlstedt]

OK, I just found your last two postings.
Now I understand.
The Hurco will do two of those passes in one block using the POCKET LEFT-POCKET RIGHT as I mentioned above
Just be CAREFUL in this Mode, as there is no Z Retract between the first and second passes---.at least not on my KMB3
When I have to do what you want in 3 passes, then it takes multiple blocks. I usually do a "COPY BLOCKS" and make dups
of everything the same , and use 3 different tool numbers , except I use the same tool.
So my 1/2 cutter is 1.500 in the first block, 1.000 in the second and .500 in the third with all cutter heights the same
Easy when you have no auto tool changer , but does require a restart
The other way to do it without tool changes or multiple tools and continuous running is the SCALE function ( X and Y only ! ) which works also if the part center is orientation center
( Rectangle works great )

Rich

[Rich Carlstedt]

Starmack
Please disregard my last post. I drove almost 600 miles yesterday and was a bit wonkey when I read the thread.
I'll leave the message for those who read this thread later.

As I said in Post # 11, Hurco does allow some of what you want in removing material that is wider than the cutter.
If you went to .150 wide cut on your example, you could do it in 2 passes on a single block and also a finish pass.

My warning on a Z axis disaster is when doing a OPEN POCKET cut ( doing a "C" shape instead of a "O" shape ie.)
The quill does not retract and you can smash into the part .
If you are outside a frame and go all the way around, it should not give you a issue

Sorry for not being clear, and I could be all wet , not having run your control ?

Rich

[starmack2001]

That's my machine with the exception of the input kyeboard accessory.

[starmack2001]

I contacted Hurco applications per Harold Cox's advice. He's the repair service rep here in the Houston area and I've talked with him for many years as I've owned Hurcos in the past. Following is the reply that the applications group sent me. I tried it on the hole that I was trying to cut and it worked. The only odd part is that the % pocket overlap setting the depth of cut is the opposite of what I thought it would be. I used 90% on a 3/4 hogging mill and it stepped over 0.075 per cut. I strated at 5% and was getting almost a full diameter cut on the mill. I would have thought it would be the other way around, according to the "help" note that comes on when I highlight the % line. It also solved a similar problem that my son was having on his hurco at his shop.

From Hurco:
If you want to take multiple passes, you will want to program your circle as an arc in lines and arcs. I would recommend breaking up the circle into two arcs, but that is not really necessary, just a habit I have gotten into. For your milling type or cutter comp, you will choose profile left instead of just left. The profile left will bring up a max offset field that will allow you to offset from the finished wall to start machining. It will then look at your pocket overlap percentage in you program parameters to see how much to step over between each pass. Remember that the percent of overlap is wanting to know how much of the cutter is overlapped, or not cutting, not the width of cut.
I hope this helps, if you still have questions, please let me know.

Jason Falk
Senior Application Engineer
CMTSE
Hurco USA
[email protected]

[email protected]
Application mail monitored by all Application Engineers

[gcude]

Remember that the percent of overlap is wanting to know how much of the cutter is overlapped, or not cutting, not the width of cut.

This seems backwards to me as well. But what do I know?