“Twisted” while Broaching 400 Series Stainless

I’m using a quarter inch hexagon broach to create a quarter inch deep form in 400 series stainless steel. However, the form is twisted, somehow spiraling from one end to the other. I don’t see any type of adjustment available on the broach holder. How can I get rid of the twist?

Spinning out of Control

Dear Spin Doctor,

The solution to removing the twist from your form is easier to find when you understand the nature of the problem. The sides of the broach include a relief angle greater than the angle of the rotary broach holder so it will not interfere with the part. The broach is held in the holder at a one degree angle. The rotary broach is designed to cut a form into the part using a cutting edge with contact points that are constantly changing. The center of the cutting edge is always kept in line with the axis of the part. As the contact point continually changes, separate chips develop in each corner of the form. As these chips increase in size, pressure is absorbed by the broach tool and tool holder. This resistance against the broach holder spindle and bearings may cause the broach to drag slightly against the material being broached. The sides of the broach cannot hold it straight because they have a greater relief angle for clearance and sometimes a spiral will develop along the length (depth) of the form.

At first you may have noticed that the form appeared smaller at the bottom. What you are really seeing is the sides of the form following this spiral path. Although there may be a slight twist, the part may still be within specification. Technicians will often recommend that you broach to the high side of your tolerance for this reason.

Work piece material can also affect this condition. Some materials could be too tough or too hard for the capabilities of the tool holder. Your material (400 series stainless) is difficult to broach, and may result in poor tool life. The combination of a dulling tool and hard material increases the thrust required to broach which increases drag thus increasing the spiraling of the form. However, at this small size and form, I’m hopeful that there are a few things you can do to try to reduce or eliminate the spiral.

First of all, good broaching practice is to check your tool holder and broach to make sure they are on center. If not, re-center the tool holder. If you are using an adjustment free model, make adjustments on the machine to assure that the broach is on center with the part. It is also good to check and make sure the pre-drilled hole is on center. Next, anything you can do to reduce the pressure caused by chip accumulation will help. Check your pre-drill diameter. Can you make it larger? The recommended pre-drill for a hexagon is 1.035 times the across-the-flat dimension. The standard quarter inch broach is likely .253 inches, and the pre-drill should therefore be .261 inches. If your customer will allow it, make the pre-drilled hole larger. This will reduce the required thrust. Have you checked your speed and feed to compare them to the recommended settings? If your tool is moving too slow, the chip may not curl over as readily as is necessary and this could result in added pressure. Increase the feed rate to improve the chip flow.

Finally, if the above recommendations do not help or are not practical, reverse the direction of the spindle at half of the depth. This will drag the spiral in the opposite direction and can reduce the overall deviation by half. Hopefully, these suggestions will help you make a turn in the right direction.

Peter Bagwell
Slater Tools Inc.

Peter Bagwell is an engineer at Slater Tools Inc., which specializes in rotary broaching tools. For more information go to www.slatertools.com

Avatar

About Peter Bagwell

Peter Bagwell is a Product Engineer at Polygon Solutions. For more rotary broaching information or technical support, visit http://www.polygonsolutions.com

Share this post

6 thoughts on ““Twisted” while Broaching 400 Series Stainless

  1. AvatarMichel Albert

    To add a comment to Mr. Bagwell I had a different problem but the solution could be the same. Spline broaching in Aluminium 6061-T6 1 ½” Dia. the tool holder back off . The solution was that the wear of the bearings , it’s very important to be changes frequently, and greased each 2 hours of productions.

     
  2. AvatarPeter Bagwell

    That’s a great point Michel. The holder must be greased every couple hours on a constant run. Also, if the improper grease is being used, it could cause the bearings to get sticky and the spindle of the holder will not rotate properly.

     
  3. AvatarDon Taylor

    Hi guys. I agree pretty much with the consensus but would like to highlight a couple of points. First, if you are running on a screw machine it is likely you will not be able to reverse the spindle. The hole size is critical as is the feed rate. I have seen a lot of machinist assume that with the harder material they should slow the feed rate. If you attempt to feed too slow the material can work harden causing your situation. Once that material begins to “flow” it need to keep flowing at a steady quick rate to avoid that work hardening problem/
    Hope this helps.
    Don

     
  4. AvatarMatt Dahms

    if you run the broach counterclockwise in about half way then change direction to clockwise this will eliminate your twist.

     
  5. Avatarclocdoc

    The holder must be greased every couple hours on a constant run. Also, You need a high temp grease in the bearings.The hole size is critical be shure the drill is not worn on sides and hole is undersize. I have put broach in aux sIide to control the feed with cam rise.I have seen a lot of assumetion that with the harder material they should change the feed . I have also honed a small flat holding broach on a hard stone.Center line of the broach is very inportant the recomended length must be held for holder size. Also the broach must be to center line of the hole. I am a former screw tech. of 30 years.

     
  6. AvatarPolygon

    Another trick is to englarge the hole slightly below the face of the part. If you’re just putting in a hex for a wrench, you don’t always need to go the full depth, and this eliminates alot of material removal. Basically you make an oversize or tapered undercut.

     

Comments are closed.