CNC Router Gouges in High Temp Foam

[Ployd]

I was cutting some high temp foam and noticed some small gouging marks in the surface of the foam. It appears to be gouging in the direction of the parallel cut. And it only appears in areas where there is a steep wall where the cutter is diving or rising quickly. The rest of the surfaces came out great. I was running a finish parallel toolpath with a 1" spherical cutter at a 0.025" stepover. Any ideas on what might be causing it would be appreciated. We have a 5-axis Quintax router.

 

Thanks, Bill

[ERIC14779]

I also have a Quintax and I think your problem is that you are driving the machine too fast for moldmaking.

 

My bridge is 48" and even though a quintax is many times stiffer than a thermwood or motinmaster, It is still 50 plus inches from the bridge rails to your tool tip...

 

That is a long lever and the Z axis weighs about 400 lbs.

 

also in corners you are getting chatter as the tool gets buried. spindle speed adjustments help.

 

I usually run ours at about 80 to 120 IPM for finishing a mold. I have done many aluminum molds on ours as well you have to adjust speeds and feeds to get the finish you want.

 

Just remember a Quintax is still not a machine tool... It is a router. that is much better than most.

 

for comparison look at a VMC of the same work area and see how big and heavy it is.

[Guest SAIPEM]

I hate to burst your bubble but a CNC Router IS a Machine Tool.

 

Most routers simply aren't designed to cut metal.

 

PS- 120 IPM is incredibly SLOW for mold work.

[Jimmy Wakeford from Barefoot CNC]

Ployd, I agree with Eric that what you are seeing is "flexing" due to the length of the z axis combined with direction changes.

 

Couple of things you may want to try is the high feed option or using the new hst paths.

 

The high speed option will accomodate the driectional changes according to machine dynamics and acc/dec by changing the feed rate to go slow where it needs to and flat out where it can.

 

The hst paths will do some toleranced smoothing of the path enabling higher feeds without as much "flex".

 

Look at the "highfeed optimization" and high speed" vids here:

http://barefootcnc.com/videos.htm

[Rick Henrickson The Boeing Co.]

Ployd you answered your own question, we have a Quintax. Not being mean but they are not very rigid routers.

[ERIC14779]

Rick,

 

They are better than Thermwood or Motinmaster

 

and for $170K for 60" x 120" x 48" real cutting area. they are pretty dam good !!!

 

what brand are you using ???

 

 

SAIPEM

 

What I meant was that all "routers" are not built like a MACHINING CENTER AKA Machine Tool. yes they are driven by CNC but they are not built with cast iron and weigh 30 to 40K lbs.

[Thee Starry™]

quote:

---

They are better than Thermwood or Motinmaster

---

You say that like there are machines out there that aren't!

[ERIC14779]

Starry69

 

LOL

[steve f]

Ployd,

 

a good rule of thumb for 3D surface machining is to use z-level type cutting on steep surfaces and not drive a toolpath vertically because of the problems you're encountering...the same thing will happen on a relatively rigid VMC cutting tool steel because the tool is getting pulled into the material as it travels down and pushed away from material as it travels up.

 

HTH,

 

steve

[Ployd]

Steve,

I'm not following exactly what your saying, as far as, z-level type cutting on steep surfaces. If you could elaborate I would appreciate your help.

 

Jimmy and Eric,

We are running 400ipm at about 60-80% We have also been using HST and I think that is a better way to go. I'll watch the videos and see if we are missing something in the HST. It is high temp foam so flexing could be an issue but we were on a finish pass and only removing 0.05" of material. Maybe it is the weight and speed causing the flex.

 

Thanks!

[Rick Henrickson The Boeing Co.]

Eric we have quintax and cincinati

the quintax column is just so wimpy.

there is a new router out craneu I am not sure on the spelling but they have pretty nice machines that are alot more rigid

[Colin Gilchrist]

Hey Guys,

 

The other thing to look at is your surface tolerances...

 

In the "Finish parallel parameters" page, click on the "total tolerance button".

 

What are your settings?

 

The filter tolerances have been discussed many times. Do a search for these keywords: surface, filter, tolerance

 

Here is a basic rundown:

 

Filter tolerance: This is applied to the calculated toolpath AFTER the toolpath has been calculated. This setting reduces the amount of G-code that is output, based on your tolerance value.

 

Cut tolerance: THE MOST IMPORTANT for what you do. This determines how accurately the toolpath is calculated. All of these values are bi-lateral, meaning that the tool can vary from the surface ON EITHER SIDE (+ or -). So if you have a cut tolerance of .0005, your total cut tolerance is really + or - .0005.

 

Total tolerance: this is the combined tolerance from both the Filter and Cut tolerances, again, this is a + or - value.

 

Try this, use the 2:1 ratio setting and set your cut tolerance to .0002 and your filter tolerance to .0004.

 

What kind of control is on the Quintax? You might have the option to run un-filtered code and let the control on the machine filter it for you (this works well depending on what your control is capable of).

 

HTH,

[Ployd]

Colin,

 

We use a filter of 3:1 and then change tolerance to 0.0005 and we uncheck the 3 boxes. We have a xxxxor. But we just found that our B-axis gearbox needs to be replaced. We just ordered a new one.

 

Bill

[ERIC14779]

Rick

 

A Cincinnati is not in the same realm as Quintax and the like.

 

Cincinnati makes machining centers Mills lathes ect.

 

I bet the Cincinnati machine weighs 5 times as much as the Quintax.

 

check this link

 

http://www.cincinnatilamb.com/5axr.html

 

is this what your cincinnati router looks like ??

 

does it rapid at 1000 IPM and can cut at 800 IPM ??

 

I bet it cost WAY more than $170 K