Couple of simple WinMax questions

[Captdave]

One of the first jobs I'm planning will be thread milling a series of 13 studs that will be held vertically in one fixture between two vises. When using a chamfer mill, will the conversational software take in account the shank diameter when chamfering the OD of the part just below the threaded area to avoid interference? Example; the shank of the stud is .580 and the thread is M10 x 1.5. If the 3/8” cutter cuts at the very bottom of the chamfer mill it will interfere with the threaded area. It seems that by properly describing the shank of the tool in tool set up should calculate an appropriate off set clearance distance. Is this the case or is there something else I should be aware of?

I also need to add a hexagon just below the threads. The hexagon pattern in milling seems to be for pockets as opposed to an OD. Is there a way to modify it for this purpose or do you have to use lines and arcs and describe each line segment of the hex?

Is there a simple command to move the table to a point after machining to load/unload parts?

Thanks in advance for your input.

[Captdave]

I did find the position soft key in part programming for end of program positioning moves.

Anyone have advise on the other 2 questions?

[glovebox20]

Hello.


To me it sound like you want to take a 3/8 dia cuter with a 45* point and drop it down to the bottom the the threads (M10 threads on top, .580 Dia below the threads) and put the chamfer down there and not on top of the part. I would call the cutter a 3/8 EM and use .380 (add .005 for clearance) for the Dia. and Adjust your Z depth to your total hight of your point + your distance down and program to go around your Threaded dia if touching the tool off on the bottom. If you want to use the same tool to chamter the top of the part, I would pick my Z depth and adjust the Circle dia. until I get what I want.

I'm not real familiar with the hexagon pattern. If It's under the same Pattern menu as pattern Linear, Rotate, Location, mirror etc., it's probably best use for making "copies" of or program blocks and translating them to a different spot. I would mill the "hex" using lines and arcs (don't forget the use "blend arc" to break the corners). When you get that done, I would create a "pattern Locations" block and enter the location where you want to mill the hex.

Mill 5/8 out side hex example

Part Zero Center of part
Tool 3/8 EM
The top of the hex will be at 0* (straight on X axis)
Use Mill lines & Arcs and cut "Left"
All dimensions in inches

Segment 0 start: X-.5625 Y.3125 May want increase/decrease X to so EM dose not plunge on part or cut air for too long. Y start 1/2 of hex (across flats)
Segment 1 line : Leave X&Y blank, type 0* for angle of line.
Segment 2 Blend Arc: .010" or what ever you wish to break corner with.
Segment 3 line: X.3608 Y0 Angle 300* (X=total distance across hex dived by 2)
Segment 4 blend arc: .010"
Segment 5 line : leave X blank, Y-.3125 Angle 240*
Segment 6 Blend arc: .010"
Segment 7 Line: Leave X&Y blank, Angle 180*
Segment 8 Blend Arc: .010"
Segment 9 Line: X-.3608 Y0 Angle 120*
Segment 10 blend arc: .010"
Segment 10 line: X Blank, Y.3125 Angle 60*
Segment 11 blend arc: .010"
Segment 12 Line X-.160 Y blank Angle 0* Adjust X so there enough "Line" to complete the Blend arc move (Tip: check X end in Blend Arc segment & adjust X on line segment)
Segment 13 Arc: CCW X blank Y.344 Radius .312 This will pull cutter .032 or so off part before moving up. May need to add the full .312 on the Y end (Y=.6245) followed by another line at 90* if milling a undercut to get cutter away from part.

The "blanks" should fill in with the auto cal. function once there is enough info for Winmax to calculate the missing values. You will have the Trig out the widest point on hex (segment #3) or pull it off a Cad system if possible. You can use Pattern Rotate if you want to change the angle the hex is orientated at.

I wrote this Program in my head without using PCMAX or Winmax but It should work but no gauntness are applied.

I easiest way I found to position the the table is to find your Part zero, the Jog the machine where you want it to load/unload the vise. Write the position down. Go back to your program and create a position block. Use the tool from the previous block and enter your X,Y position. Leave the "Position Stop" to "NO" to avoid having to press cycle start twice to restart the program. As a bonus, you can program another position stop block at the end of program (using the same X,Y) using the first tool in the program so machine will "home" the spindle, position the table, then change to the first to in the program. If you wanted to add a program stop in the middle of the program, Put a Position Block where you want it to stop and select "Yes" for "Position Stop"

Hope this helps

glovebox20

[Captdave]

Thanks for the program example, I'll plug in the numbers next week when I get back in town and see how it works out. The Hexagon pattern I'm referring to is in the milling section, maybe I'll try using it as a pocket with an island and see if I can make it work that way.

Thanks for your input!

[Captdave]

Segment 0 start: X-.5625 Y.3125.. shouldn't the X be positive?

[glovebox20]

You can try a X positive on segment Zero, but you will find out that it won't work.

Remember, Part Zero is in the center of the shaft. All dimensions are absolute. Top of the hex is straight to the X axis. All X dimensions to the left of zero are negative and all X dimensions to the right of zero are positive.

I'm starting the EM on the upper Left corner of hex and milling around the outside of the hex in a Clockwise motion (climb milling-"cut Left"). Segment 1 takes the end mill from the Upper left corner of the hex and mills straight across moving to the right (Angle: "Zero") until it reaches the upper right corner of the hex. Then I keep milling around the part using lines & arcs until I reach the upper left corner where I started and arc off the part before moving the EM up. If you were to start segment Zero with a positive X, you would be starting on the upper right corner and segment 1 would have mill down to the right at a 300* angle until it reaches the right center corner of the hex. I picked milling the top line first at 0* to make it easier to program. I did run the program through a Ultimax control the other day and it appeared to be correct on the graphics screen.

Hope this clears up your question.

glovebox20