Milling: Cutter compensation & lead-in/out arc

[SlaveCam]

Hello...

 

With every single different Mastercam installation/version I have ever tried, I have never been able to get "arc" lead/in-out to work when cutter compensation enabled in control. It works when only straight lead in/out is enabled. What I'd like to have is: enable cutter compensation with G41/G42 with a linear movement, then do the arc movement with compensation enabled. 

 

 

What's the catch? 

[Oppiz]

It might be something in your post

[Colin Gilchrist]

The catch is that both the arc and the line length must be greater than 51% of your endmill diameter.

 

Try using 60% for both arc and line, and it will work. It also shouldn't matter if you program "tangent" or "perpendicular", as long as you are greater than 50% of the diameter...

[mmoya]

I too am having this problem. Got a alarm 357 cutter comp interference because the arc was 50%. Changed lead in/out arcs to 100% and didn't get the error. BUT- when we ran the program, the machine ended up taking a huge bite out of the side of the part that should have been a .003" finish cut... My mistake is I only backplotted instead of simulating, but the issue is still not resolved... This is the first time we've ran control compensation.

 

It looks as if the cutter is following the toolpath at the center of the tool during lead in/out, and at the end of the lead/beginning of toolpath, it switched to cutting edge...

 

[Rick46]

I too am having this problem. Got a alarm 357 cutter comp interference because the arc was 50%. Changed lead in/out arcs to 100% and didn't get the error. BUT- when we ran the program, the machine ended up taking a huge bite out of the side of the part that should have been a .003" finish cut... My mistake is I only backplotted instead of simulating, but the issue is still not resolved... This is the first time we've ran control compensation.

 

It looks as if the cutter is following the toolpath at the center of the tool during lead in/out, and at the end of the lead/beginning of toolpath, it switched to cutting edge...

 

Capture.PNG

 

make sure you have gouge check box ticked so you get no gouges on lead in and outs..

[gcode]

are you using control comp or wear,

wear is much more reliable.and you can use small efficient lead in/out moves

[mmoya]

Ah, a new day. Let's see if i can convince mcam to play nice today.

 

make sure you have gouge check box ticked so you get no gouges on lead in and outs..

Gouge check is selected, deselecting has no effect either....

 

are you using control comp or wear,

wear is much more reliable.and you can use small efficient lead in/out moves

We're using control comp because the WIPS system on our VF4 has automatic tool probing, but it registers the tool diam in the actual diameter column rather than adding a wear offset. If there's a way to change this, I'd much rather run wear compensation.

[djstedman]

I use control comp all the time because our machines also use full diameter for the offsets.

 

You should be able to get control compensation to work reliably by doing the following..

 

1 - Put in the values that you would want for line in/out and arc in/out as if you were using wear comp

2 - Add 50% of the cutter to your initial values from step 1 to compensate for the movement the machine will make when it turns the comp on

3 - Set line in and line out to perpendicular

4 - Make sure gouge check is on.

 

You will also want to make sure that backplot and verify are setup to simulate cutter compensation in control.

 

For the classic backplot, this is a checkbox you can check once you have hit the exclamation mark icon to open up options when you run backplot, for the new backplot and for verify this option is available when you hit the backplot/verify button next to the verify button on your toolpath manager.

 

Also, you will want to verify that your control definition has the control supports cutter compensation in control box checked on the cutter compensation page of your control definition.

 

Someone said earlier in the thread that the lead in or out can be set to tangent or perpendicular, however in my experience tangent lead in/out does not always work correctly, I have yet to have a problem with perpendicular.

 

Given that the arc in/out is what actually leads onto the part, the fact that the line is perpendicular should not really ever be an issue.

[jlw™]

I use control exclusively as well. If you et the parameters correct the exact same path will work for control as wear. Regardless of how you activate it cc needs the same motion. Unless I need more I usually set everything at 51% as a general setting and adjust if I need more or in some cases less.

[gcode]

It has been years since I ran a Haas, but I recall there were settings that controlled the behavior

of CDC.

Couldn't hurt to review them, perhaps something is not set up properly

[mmoya]

So update...

The problem has been corrected; BUT, I still don't know what caused it. I tried everything that was suggested and nothing seemed to fix it. I moved the starting point from the left edge of the contour to the right edge, just to see what would happen, and it magically worked! Moved it back to the left and had the same problem. I guess MCAM just didn't like it... Part is done though so I'm happy!

I'll take most of your guys' advice and stick to Control comp and see how things work out. Our last mill was pretty much a "base line" 2007 TM2, so we're still getting used to the bells and whistles of our new VF4!

[CJep]

Check your posted code, if you have a G41/G42 comp call in a G2/G3 line that is what's messing with the comp at the machine.

It's the G1 linear move that needs to be more than the radius of the tool when running in comp control.

I set my linear move in the lead in/out to 55% the arc move I've run at 25%, I also set my linear move tangent then adjust the sweep to fit the lead in/out.

 

If you have only arc on/off set in the lead in/out this will cause the code to output with G41/42 comp calls in a G2/3 line.

 

As stated earlier wear comp is much more forgiving.

[AMCNitro]

Thats a problem with Haas machines.  The way you get around it is you use both straight lead in and radius lead in.  So the tool goes in straight for a bit and then it goes into the radius and machine wont alarm.  I figured it out by chance, I had it happen with one toolpath but not another one and just looked at what was different on the mastercam side

[ahaslam]

Changing the post isn't really a good idea because it is easy to turn off the CC all together. Some times you just have to get down and dirty and visually inspect your lead in. If your leading in to a small pocket with a large tool there may not be enough room for the lead in, MasterCAM will default to no lead in. Some times you can make the lead in smaller and get something to work. Every one says they go with 51% but that doesn't mean you will have enough room to do it. some times going with a 20/10 will do the trick or even smaller. Just get used to eye balling your lead in as soon as you create it to make sure it looks good.

 

Another thing to keep in mind is your start point. If your start point is in the middle of an arc and you have start at mid point turned off then it can have a hard time creating reasonable geometry for the tool path. Try moving the start point to a different line.