Tooling marks Buddy Prs

[cowboy1296]

I know that there are other threads on here regarding tooling marks but i could not find any that i thought related to my problem.

I have started getting tooling marks while doing 3-d finishing. I cut against the grain but dont think that is a problem and that is generally in the Y direction. I use 8-10% step over and 3 inch per second feed and plunge. My plaques are typically 18 inches tall and the marks are spuratic when and where they are seen but they tend to run the full height of the plaque. My 3-d cuttings are not as smooth as normal. These marks are easily sanded if you can get to them. My last carving, when i was about 2/3 way though with it, i cranked up the rpms and the markings were still there but not as noticeable.

All pinions were replaced recently. The Y motor had gone bad and had to be replaced. All pinions feel tight and they were recently cleaned.

Any help would be greatly appreciated.

[Martin Reid]

Cowboy

When was the last time you renewed your collet? (and/or collet nut)

Sincerely and in good faith
Martin

[Gary Campbell]

I would lean towards backlash in the Z rack to pinion or static bumping the Z motor a few steps.

With a dial indicator on the Z axis extrusion pry up lightly with a 1 by 2. Does it move more than a few thousandths?

Next cut that you see this occurring on, pause, remove dust collection, resume and see if that helps.

[cowboy1296]

Collet, whats a collet. I have a cutting to do tomorrow and i will look at all options plus changing the nut and cleaning the collet. Thats for your thoughts

[srwtlc]

Since you changed out pinions of late, be sure the pinion set screws are tightened properly and that you have the motors tightened into the racks with firm hand pressure on the motor, not clamped or pry barred into the racks. Excessively tight pinion to rack adjustment can cause issues of cut quality and possibly lost steps. If too loosely ajusted, it can allow backlash. As Gary stated, check for play/backlash in the Z. Check for play in the Y car and adjust the lower rollers as needed. If there is, it may not show in 3D cutting, but it's good practice to check the Y car to gantry adjustment from time to time.

Since you have a buddy, be sure that there is no issue that could cause your table to lift slightly. Foreign objects on rollors/v-wheels etc.

[jerry_stanek]

when you run a surfacing program do you get any ridges

[Martin Reid]

Collet, whats a collet. I have a cutting to do tomorrow and i will look at all options plus changing the nut and cleaning the collet. Thats for your thoughts

Collets...
Collets.jpg

I change my collet regularly, you will be surprised what a difference it makes.

Especially if it is producing 'shadow marks' on your cutters.
bits from bad collets.jpg

I apologise if I didn't reply in time for your cutting - middle of the night here.

Sincerely and in good faith
Martin

[cowboy1296]

thanks i will look for the marks

[Brady Watson]

I have started getting tooling marks while doing 3-d finishing. I cut against the grain but dont think that is a problem and that is generally in the Y direction. I use 8-10% step over and 3 inch per second feed and plunge.

Cutting against the grain is generally a no-no. Try to always cut in the same direction as the grain. 3" per second is too fast for this, especially if you have not done a proper 3D rouging pass over the entire plaque first. You'd be surprised how much cleaner your work will look when you first rough out, then slow down the cutting speed to something like 2,1.

It pays to check your speeds in your mind's eye, imagining what is actually happening at set speeds. Depending on your VR settings, it is likely that across an 18" surface with raised letters, that the tool is almost never reaching its set speed of 3" per second. Instead, the software is trimming off the speed for accel/decel and in fact, causing the tool to make sharp, clunky moves. If there is a volume of material that was not removed by roughing, it is pretty touch on the mechanicals and router to plunge right into material at 3 IPS.

Just for the heck of it try roughing, rastering with the grain and slowing the speed down to 2,1. You may find that it doesn't take much longer than setting it at 3,3 & cuts will be more reliable with less chance of losing steps on a Standard machine. The inherent nature of steppers is that they have more torque at lower speeds than higher speeds and 3 IPS is where the torque on those motors really starts to fall off sharply.

In my experience, 3D takes as long as it takes when the bottom line is quality. I won't put my name on something that looks like I carved it out with a hatchet. If you want high quality & less hand work...slow things down.

-B

[cowboy1296]

Gotcha. I use to always cut with the grain and then would spend a large amount of time cleaning fuzzies. Cutting against the grain, i have almost zero fuzzies. for VR settings i am using what i believe is your suggestions. I know that a lot of people dont use a roughing pass but i do. Currently my machine allowance is at .013 and i may even trim that down some more.

Currently I am cutting the finishing pass on a piece which has been running for over an hour now. From what i can see, there is a major improvement. The machine does feel as if it is clunking but barely so i will slow it down in the future. I have received recommendations in the past that suggest that the feed rate should almost be identical to the plunge rate, but yours is different, but you should know best.