Mill Tips and Tricks

[Bob W.]

Here are a few tips I have had to give in the past to green employees...

 

Make sure you tighten the vise on the work piece before hitting cycle start (said about 10 minutes too late)

Make sure the fixture is actually bolted to the table before hitting cycle start (same as above)

DO NOT put tools in tool holders and just leave them finger tight, I will assume they are tight...

If you put a tool in the machine, you had better set the length or you might get fired. Don't just walk away and leave it with no offset.

When the torque wrench goes 'click' it means the part is tight and there is no need to keep cranking until the bolt actually breaks off in the fixture...

[The_kid]

lmao man things I do an not even think about that seem so obvious. These are great things to beat into a newbie's head! I've seen every single one of these. do not over tighten the vise. Oh seen someone not lock the chuck of a surface grinder....

[LancoUSA]

When I first started, I think I crashed about everything I put my hands on. Thankfully I worked someplace that I had multiple opportunities for mistakes, benefit of working for a large company. I learned fast though. Now I have 16 years, experience. I see the new guys doing the same stuff I used to do.

[Rotary Ninja]

LOL! Now that is when you know you're having a bad day. That is when I head out for a long bike ride...

 

Must be nice being the boss

 

When I first started, I think I crashed about everything I put my hands on. Thankfully I worked someplace that I had multiple opportunities for mistakes, benefit of working for a large company. I learned fast though. Now I have 16 years, experience. I see the new guys doing the same stuff I used to do.

 

Been there, done that. Crashes happen. Learn from it, get over it, and get on with it is what I try to tell the new guys.

[Bob W.]

Here is a rather important one. NEVER hit cycle start and turn your back to the machine, even if it is a proven program. ALWAYS make sure the first move makes sense. 95% of crashes will occur on the very first move because a tool or offset is not set correctly. On a new program I take this approach with every tool change. First move with the new tool is the most important.

[Bob W.]

Don't face parts on a vacuum chuck with a shell mill. It may take longer, but if the chuck lets go with a 3/8" end mill the part will only be moving at 50 mph. If it lets go with a 3" shell mill it will be more like 250 mph...

 

If you put a vise in the machine ALWAYS line it up to .0002" because when the next guy comes along (me) he will assume it has been set up correctly and go about using it. If two vises are on the machine side by side, line them up to each other every time. This reduces scrapped parts in the long run and if the machine has vises bolted to the table there is no doubt they are lined up and ready to use.

[jfranya]

One thing stressed in our shop is NEVER assume a job is set correctly. That's bit me in the keester more then once. Better to double check it for yourself than to assume someone else did their job correctly.

[Müřlıń®]

Here are a couple that have served me well over the past.

 

I use a 12" SS .001" Starratt shim to set my tool.

 

Most of my work is mold and dies and not parts in a jig so it is mostly jobshop.

Since the shop is not climate controlled exactly and the machines are not high end, I will set my offset when I need to run that tool and not set all the tools at once. You do not have to deal with heat expansion in this way. Most of my work is 3-d surfacing and multiple ball endmills of different sizes have to be run over the same area and this will insure there are no areas on the part where one tool cut deeper than the other tool due to thermal expansion of either the workpiece or the machine tool itself. if you have to unclamp the tool and look at it, reset the offset because it will most likely not seat back exactly the same if the machine has been heated up.

 

 

I hardly ever chip the tool and the tools are within .0005 of each other. Jog the tool down on the shim while slightly moving it in and out as you hold it with your thumb and forefinger. When the tool grabs the shimstock push the tool set. Your hand is always a foot away so it is safe should you do the unthinkable and rapid into the workpiece.

 

This is just a fast way to get real close as there are more accurate ways to set the tool offset.

[Oscar R.]

Here are a few tips I have had to give in the past to green employees...

 

Make sure you tighten the vise on the work piece before hitting cycle start (said about 10 minutes too late)

Make sure the fixture is actually bolted to the table before hitting cycle start (same as above)

DO NOT put tools in tool holders and just leave them finger tight, I will assume they are tight...

If you put a tool in the machine, you had better set the length or you might get fired. Don't just walk away and leave it with no offset.

When the torque wrench goes 'click' it means the part is tight and there is no need to keep cranking until the bolt actually breaks off in the fixture...

 

 

This one reminds me of a place I worked at long ago.... and for a short period of time, I might add.

The setup guys would borrow set screws from other toolholders, (becuse the lame bosses were to to cheap to buy new ones when the setup guys stripped out the old set screw... yeah...)

but they'd leave a tool in the toolholder they borrowed the set screw from. Along comes another setup guy, sees a tool already setup in a tool holder, does'nt notice(or check) that the set screw's missing and put's it in the machine....

Hey dude, what's that noise coming machine #5?....

 

You shouldn't have to, but enless your shop has a good system in place with good people, double check everything.

[MotorCityMinion]

"In my opinion that button has no business being there, especially where it is."

 

LOL, I've dented a few parts in my time.

 

Same crap on our Makino. You have to press the spindle STOP button to release the orientation after a tool change. This button is right next to the spindle start button, and both are above the control. The only 2 buttons in that location. I'm standing at my machine right across from the Makino when I hear that oh so familiar THWAK. Look over and the guy is as white as a ghost. Last programmed feed was 18500 rpm. It's not funny at all, quite serious actually. Every time i see this happen, the operator looks around for the pieces, hoping for just a bit of luck that the Interapid can some how be put back together.

 

I've managed to piece several axial supports back together after a few years. It usually takes 3 or 4 accidents to make one good one.

[Rotary Ninja]

When running a ballnose endmill over an OD contour for example, with a surface finish toolpath such as a flowline, always start at the bottom when possible. This will keep the center of the ballnose from doing any work. Starting from the bottom will always side cut the material away and leave less for the center to do...

 

If you start from the top and you have roughed the surface with a flat endmill leaving the familiar stair-step pattern you will see galding at every step where the finish tool buries the tip of the ball into the heavy part of the step as it is below...

 

Also, using a surface finish toolpath and cutting from the bottom up is a good way to not even need to use a surface rough toolpath to begin with. I rarely ever use surface rough parallel or contour toolpaths. If you do have to rough some material off first, try this same finish toolpath, but use a flat endmill staying off the drive surfaces by .030" or so. I have taken a 2" LOC in one pass this way stepping over .050" per pass.

 

 

This was done with one pass, and the deepest LOC was 2"...

[MotorCityMinion]

That works well and is how I prefer to do it. Also note that you can get some good feeds going if you apply radial chip thinning on a parallel style tool path.. I also create dummy drive surfaces around the perimeter when needed to stop that first pass from being to aggressive or force a tangent entry.

[Brewster]

Excellent post Rotary. I would like to see more programming tips. It seems everybody has a different way of doing things. I learn something new or at least a different approach every time I look at the forums.

[Rotary Ninja]

I'll trow together a couple more tonight if I get time.

[mx247]

Lots of good tips guys. New to the forum, I've been machining for over 20 years but fairly new to Mastercam just trying to find as much info as I can

[Rotary Ninja]

Welcome to eMastercam. There are some good peeps here that love to help.

[Jayson Kramer]

MotorCityMinion do you ever use the option in surfacing of Direction to control the entry and exit of the tool?

[jfranya]

Lots of good tips guys. New to the forum, I've been machining for over 20 years but fairly new to Mastercam just trying to find as much info as I can

Welcome to the forum and to Mastercam. I'm kinda in the same boat. I've been working with Mastercam since September 2012. You will find pretty much any help you need here in these forums. Unfortunately, not a lot of help from me... I'm a NOOB.

[Rotary Ninja]

Surface Finish Project:

I will show you one of my methods for using this toolpath. I am sure there are better ways to do this, but this is what I have learned on my own. And I have had some good results from using this method. I have used this toolpath a lot because it allows me to create a path that follows geometry that I create over an irregularly shaped surface such as this one:

 

This may seem like a long drawn out process but I am used to it and can create a path like this in just a few minutes on some really complex parts.

 

I am only going to show you a finish toolpath with a .020" stepover using a 1/4" Ballnose Endmill. This could also be used for the Surface Rough Project Toolpath as well. This is just one way to use the Surface Project Toolpaths. There are many ways to finish this surface. But this would be my favorite way because as you will see the toolpath follows this contour exactly.

 

Start by creating a line along the ends and along one side of the contour you wish to follow like the red lines below. I usually draw this a bit above my part to give some clarity.

 

Since I am using a 1/4" Ball Endmill I offset the geometry on the ends by .260" to give the endmill room to extend over the end of the part. I offset the first chain along the side of the contour by .240" to force the first pass to take a .010" cut. Then trim the contour to the lines at the ends.

 

Then delete these ends (yellow geometry) becuase they are no longer needed.

 

Select Xform>>Offset Contour and select the chain

 

This flange is .500" wide. Since my initial cut is .240" from the edge, plus the .500" thickness equals .740" distance I need to travel. I am going to use a .020" stepover just for this demonstration. So .740" divided by .020" equals 37. So offset the geometry by .020" - 37 times.

 

After that draw a line across the ends of the geometry and use the Trim Divide tool to delete the line between every other path on each end. NOTE: On the opposite end of the path you need to delete the opposite lines so your path creates one continuous chain across the part.

 

Select Toolpaths>>Surface Finish>>Project. Select the drive surfaces (blue)

 

Click the curves button

 

Select the chain you created.

[Rotary Ninja]

And after selecting a 1/4" Ballnose I left all of the default settings alone and got this...

[Rotary Ninja]

There are a couple benefits of this toolpath. It never stops making chips for more than a second or so as it wraps over the end. And it follows the contour you draw. So if you want to write your name in a part with the toolpath you only need to draw it...

[Jayson Kramer]

RN can you send me the model of the shape of this Project path you are showing. I would like to add some thought.

[Rotary Ninja]

That would be awesome. All I have is the HLE though. I assume you can open those. I'll email it to you.

[Newbeeee™]

Kev - keep up the good work

When's your book coming out

[Rotary Ninja]

As soon as Jay gets done editing it LOL