Cutting grooves in thread format

[Thoob]

Hi guys, I have a part that has basically a thread on it but instead of the thread being 60 degrees, its a square groove instead. Now I don't have a problem putting the path to the part using a diameter and a pitch that I measured(by the way,I only have part for sample, no drawing). The problem I have is that the groove width is .200 and I only have a 5mm groove tool. Is there a way to make the width wider but maintaining the pitch? Or do I have to do a Z offset and run the same cycle over? By the way the groove depth is .035.

[crazy^millman]

Thoob, you answered your own question. I use to make a 7 pitch acme and could never get the custom insertes for it. I did it just like you are talking about doing here. Be careful that insert is not really made for threading might need to take light cuts ot aviod to much side load on the insert.

 

HTH

[Thoob]

The insert is an Iscar Heli Grip. It definetely can turn and thread. Now I guess that introduces a new problem. I have 80 parts to make. Is there a way to add the z offset into a program instead of manually changing offset each part?

[K2csq7]

I would program 1 pass in the middle, then a .002 stepover each side...

Or, considering you have 80 parts, rough/finish 1 side then a .004 step to the other side and see how the tool reacts, Heli Grips stay damn close to where I put them so I wouldn't be concerned about deflection....

[Thoob]

I would program 1 pass in the middle, then a .002 stepover each side...

Or, considering you have 80 parts, rough/finish 1 side then a .004 step to the other side and see how the tool reacts, Heli Grips stay damn close to where I put them so I wouldn't be concerned about deflection....

 

Thats what I'm asking how to do. How do you program like that?

If I just select in the parameters a different start and end point, would it start the thread at the same orientation or would I risk the second thread starting somewhere else?

[crazy^millman]

Today not like the past we had to worry about that, but today, just call the same thread cycle with different tool offset. You can have the same lathe tool with 10 different offsets. Use them to help you make the thread. Call the thread cycle 5 times in Mastercam just using different offsets for the tool number and done. Control at the machine and you should be good to go.

[K2csq7]

Are you concerned about your spindle syncing up to the same spot?

[Thoob]

Ya thats what I was concerned about. I did offset the nessessary length and ran a couple sample parts in aluminum and the spindle synced (sp?) the same spot. Wasn't sure if that would have been a problem. Thanks guys.

[K2csq7]

Ya thats what I was concerned about. I did offset the nessessary length and ran a couple sample parts in aluminum and the spindle synced (sp?) the same spot. Wasn't sure if that would have been a problem. Thanks guys.

I was going to say run a test part.... Glad it syncs up for ya!

[Tim Johnson]

Call up your customer to find out how important the .200 width is. The part may have that thread there for use as a spark arrester, impeller or something similar.

 

You may need to grind relief on the back side of your insert. .035 deep isn't much though.

[Ivan Mikesic]

There is an option to have your post modified that would allow you to use the groove toolpath to cut this thread.

 

Two misc reals are typically setup to control the retract from the thread in X (between points) and to set the length of the thread in Z.

 

Each cut position in the groove toolpath outputs a G32 with the length of the thread. It retracts to the X value set in the misc reals, then moves to the next point and continues.

 

For this type of post modification, I would recommend contacting your reseseller.

[Thoob]

Call up your customer to find out how important the .200 width is. The part may have that thread there for use as a spark arrester, impeller or something similar.

 

You may need to grind relief on the back side of your insert. .035 deep isn't much though.

 

The part is a drill end adapter. The sample I got was in rough shape. I asked about tolerances and important dimensions when I got the job and they told me just make it as best you can to the sample. They just want it to thread in like the sample. So I did just that. I'm not worried about the .200.