Project-Surface toolpath. Problems?

[TK-32™]

Hi guys, I'm have a problem using the Project-Surface Toolpath. Everything looks ok on Verify but when I run the program on the machine it does some weird stuff and cuts where it's not supposed to. On The image below you can see the part on Verify and the .500 wide detail. At some point both the roughing tool and the finishing tool do what it seems like a full circle on the G18 plane. That's when it crashes in to the part.

 

 

 

 

I'm running X2 MR2 SP1. At one point I thought it was our old control's buffer. I had this same problem on an older machine but different part. That time I changed my toolpath. I wonder if I'm doing something wrong. I don't do much surfaces.

Thanks in advanced

[TK-32™]

code:

---

 G3X7.3369Z-.6476I-.1134K.4207

G1X7.3351

X.5449

X.5447Y-3.0286Z-.6486

X7.3358

X7.3376

G2X7.4503Z-.6338I0.K.4354

G1Y-3.0246Z-.6349

(G18)G3X7.3384Z-.6495I-.1119K.4205

X7.3365Z-.6496I0.K.4351 (<-----here's where it makes the "full circle")

G1X.5446

X.5445Y-3.0206Z-.6506

X7.3372

X7.3391

---

[Mark V.]

Haveing create arcs in the XZ and YZ plane checked in the toolpath filter will do that. Some machines dont handle arcs very well in those planes.

[Thee Rickster ™]

I use surface paths all the time but don't use the project. Are your clear and reference planes set to

absolute and are above your workpiece?

[TK-32™]

Mark- yeah, last time I turned the filter off but the finish wasn't as good. I might have to do that again.

 

Rick-I'll check that.

 

Thanks

[Mark V.]

quote:

---

Mark- yeah, last time I turned the filter off but the finish wasn't as good. I might have to do that again.

---

I would leave the filter on just uncheck those two boxes.

[TK-32™]

Isn't that the purpose of the filter? To create arcs instead of many lines and thus reducing the NC file size? I might be wrong

[Colin Gilchrist]

Leave the filter on, but turn of "create arcs on XZ and YZ planes".

 

That is a real bummer about the part.

[TK-32™]

quote:

---

Some machines dont handle arcs very well in those planes

---

That's what I get for cutting surfaces on a Fanuc ROBODRILL

[3R!< W3NG3R]

were you using r's instead of IJK?

 

On fanuc controls, some need a -R value for arcs bigger then 180 deg. (or something like that)

[TK-32™]

I was using IJK.

I'm using a MPmaster. I unchecked the boxes XZ YZ boxes and now it's OK. Thanks guys.

[Greg_J]

TK, do you have a program that you can view the toolpath separately from MC? Like Cimco or something?

 

I use Cimco to view all my tool paths before I post them to the machine because what MC shows and what is posted are sometimes different.

[TK-32™]

No Greg, but we're getting cool parts more often so it might be something to look into. Do you have a link?

[Greg_J]

Cimco Edit 5

 

I use it all the time to check that MC posted the program correctly, I use it regardless of the part I'm making. You might have caught that mistake if you had a external program to check the NC file.

It's not perfect but it's better then nothing.

 

HTH

[Greg_J]

Many people here use Vericut as well.

[TK-32™]

I assume that Cimco editor on MC is a water down version of that program.

[MotorCityMinion]

I thought I've read here somewhere that in X2, it's watered down. I think you get the full version in X3 and X4.

[mayday]

sad but true, MC's backplot will show a crash much better than verify. It just takes a lot of time closly watching the tool contact the model. but it works. TK. did you try backploting that area and see if it shows the gouge?

[MotorCityMinion]

Po boys verify. If working with solids, make surfaces from solid then view the path from the backside of the surfaces. The path at the tip of the tool will show on the surface and the tool itself will pop through the surface if it violates it.

[Colin Gilchrist]

Let's not get carried away here.

 

The main problem is that TK's control couldn't handle the code that was output from his Post.

 

All the backplotting and verifying in the world wouldn't have shown his particular error.

 

Cimco, Vericut, and Predator VNC could all show this error, If they were configured correctly.

 

That being said, I use MCM's method all the time (create surfaces and view tool gouging through the surfaces from the backside).

[j.nguyen]

I was bored so cut the code and inserted it into

one of my vericut files. With the controls settings that was already in place in Vericut. It drove the circle just fine. I'm guessing the control is set up to read quadants instead of 180 circles. It looks like your cutting heat treated stainless, so I guess you are not going that fast where the buffer can't keep up. If you look at the code it's swinging about a .100 circle from I.0 TO I-.1119 which would be a 180 degree swing.

[Alvaro Gil - Cimquest-inc.com]

Something you might want to experiment with further is to try making arcs in the XZ and XY plane work with that control, the machine will cut some much smoother at higher speeds.

 

Make sure allow 360 deg arcs is UN-checked and also click on the break at 90 deg button for every plane in the control definition.

 

I bet that will solve the issue.

[Greg_J]

I just meant to add Cimco as a tool to prevent mistakes. I assumed what was said about the control def not being set up to match the machine was what the problem was.

[TK-32™]

quote:

---

did you try backploting that area and see if it shows the gouge?

---

Yes I did and it looked fine.

 

quote:

---

The path at the tip of the tool will show on the surface and the tool itself will pop through the surface if it violates it.

---

tried that and no problems on Backplot

 

quote:

---

control couldn't handle the code that was output from his Post.

---

I'm leaning towards this theory.

 

quote:

---

It looks like your cutting heat treated stainless

---

bad cellphone picture. Aluminum

 

 

quote:

---

Something you might want to experiment with further is to try making arcs in the XZ and XY plane work with that control

---

I have and that's why I like creating arcs on those two other planes.

 

 

I'm starting to believe it might be a control issue. The roughing and finishing code was about 242KB with G18's left and right and it only did that 4 times.

Thanks for your input guys.