I need an expert! i am struggling with finishes on HDPE and MAPLE!!settings or motor?

Attachment 24970Attachment 24971Attachment 24972Attachment 24973Attachment 24974I purchased a used shopbot a couple months ago for my start up business. I intend to use the machine to cut out small parts from HDPE and MAPLE hard wood. I havent been able to achieve a smooth finish from the day i got it.

I am trying to product parts to a board rack called, the gnar bar. Here is my website so you can see the application side a bit more (royal-racks.com). I bought the machine to cut these pieces out of hdpe and maple hard wood. I have 4 parts I am looking to cut out of each material:



2 End caps (left and right)
1 Back Plate (mounts to the wall)
1 center piece (holds the bar to the backplate)

The end caps are to be cut out of 1" thick Densetec from Sabic (BLACK), and 1" thick Maple Hardwood.

The Back plate is to be milled out of 1/2" thick densetec from Sabic (BLACK), and 1/2" thick Maple Hardwood.

The center piece is to be milled out of 2.5" thick Densetec from Sabic, and 2.5" thick maple hard wood. ( we are milling half, then flipping to mill the rest)

What I have been using for a cutter is the

Onsrud 63-783 3/8" single flute o spiral

I have been using this for both materials and have played with a 1/4" double flute up spiral from onsrud on maple.

Again, I have not been able to get a smooth finish for the life of me, i have tried faster and slower feedrates from 1in/sec to 3in/sec with and without a finishing pass taking .03, conventional on wood, climb finish on hDPE. I STILL cannot achieve a smooth finish.

I replaced the brushes and bearings in my 7518, but we did have the worry that maybe we were getting chatter because the motor is worn out? or is it the fact that i have not found the right feedrate yet? everything i have ran has been at 16,000 rpm.

I also have an issue when i run pockets on these parts because it move the cutter so slow and then all of a sudden just jerks into full speed. I have also noticed it melting the hdpe in this case and that cannot happen.

I would really like to get on the phone and just go over everything, from feed rates, to plunge, to crossover. I need to get this thing dialed in so i can start my company and pay expenses, but i cannot seem to achieve a smooth finish. Is it the feed rate? is it the bit im using? is it my router?

also, when i do a pocket tool path, the bit sits in the same spot for way too long causing heat and melting of the plastic, is there a way to program around this or is this a cross step % issue?

are these ridges from a worn out motor? the wrong tooling? the wrong feeds and speeds?

I have included some photos of my trials, please help me, Im becoming annoyed and this is just the start, I cannot wait to get into production and custom engraving!!!

thank you very much for your time, I certainly hope you can help me in the right direction.

Thank you,

Brandon Bauer
Brandon@Royal-Racks.com
608.630.0153

What depth of cut per pass?
have you tried using a pocket that stops short of your line and then run a profile pass?
How are you holding it down? If its vibrating it will never cut cleanly.
the slow starts and stops sound like a ramping issue? Brady has posted on this.
Have you called Shopbot?

David

I have never found hdpe to cut really smoothly it is too grabby when cutting. most soft materials are like this.

Brandon,
First thing's first. That tool needs pinion gears (on X&Y to start) and the racks need to be greased. If it is a PRT model, set the spring turnbuckles @ 3.5 turns from when the spring starts opening up. This is where the rubber meets the road...If this is a PRT and you run your fingers down the rails and they feel rough - this can telegraph into the cut as well.

The other issue of the tool moving suddenly is probably attributed to the computer not being fast enough (USB communication), although it can be a problem with the VR settings not being correct. I would reset the VR settings to stock (via VR fillin sheet) after I performed maintenance on the tool.

There is no way to completely get around some edge marks in HDPE, but what you show can certainly be improved upon.

I don't know what model tool or drive system you are running - this can also affect cut quality (E.G. - 3G PRT controls are horrible on plastics - 4G much better - Alpha w/7.2 motors or Desktop best)

Single O-flute is OK, but you can't really run it efficiently over 2 IPS. A double or triple O-flute (via Onsrud) would give better results and permit higher speeds.

Question: How are you holding these parts down? (this will also affect quality).

-B

Hey Brady, thank you very much for a thoughtout response.

I am holding down 24x34 inch section by a 3/8" bolt in each corner, and the center. i cant feel any vibration while cutting, and certainly cannot budge the material. I have been making jigs out of pine creek mdf, as i am trying to run for production (just havent got there)

i own a bt-32, not a PRT

how do i know my drive system? i know this is a little bit older of a machine (2009 i think) i just upgraded my driver to the latest one for my model (it was not capable of running the latest driver update)

.375 depth with my 3/8" tool, i have left an allowance of .03 to clean up for finish, but i have not been successful in a smooth finish.

I have a solid hold down of material by bolts in each corner, and center.

I have reset my ramp values as instructed by SHOPBOT.

Hey Brady, what would you recommend for cleaning and greasing the rack and pinions? how often should this be done?

I maxed out my table to 24x34 by moving the prox switches to the max and then using the upper left corner at my "home" each time. I do this my finding home from prox switches, and then i send my Y axis to 33, and then zero all axes. Is there a better, or more consistent way of doing this since im using this as my HOME every time? i am trying to set up for productin i mind, jigs and sheets of material. i need everything to be exact so i can flip the sheet over and mill out the rest (for my 2.5" thick piece) nevertheless, i need HOME to be the same EVERY time....

Does the control box look like a desktop computer (ATX case) or is it silver/brushed aluminum?

What color are the stickers on the end of the motors? Red/Silver/Black or Violet/Gold/Silver?

There are 3 gear racks on the BT. The one on the Z (probably OK) the one on the X that moves the table in & out and the one on the Y which moves the YZ car. ShopBot uses a synthetic grease in a mini grease gun tube. Any synthetic grease from the auto parts store is fine. Put a dab every 6" and work it in. Then wipe it down. Repeat 3x - moving the tool -X, +X, -Y, +Y and wipe it down. Do this at 1 inch per second or it will fling it all over. If the gears are currently dry - you need to replace them. From the looks of your cuts...they need it on the X & Y.

Keep the racks 'wet' with grease. Steel on steel is bad. Grease slathered all over the machine is not what you want either. You can clean them with a brass or SS brush. Just rake them out.

With the machine powered up, shake the machine down. Wiggle the table in & out. The YZ car in out up down & all around. Feel for both gear lash and v-roller bearing slop. Track it down, adjust and shake it down again. You don't want any slop in the machine or it will cause chatter in every cut. Check the router mount and make sure it hasn't loosened up.

The BT has more slop in it because of the moving table. You want to make sure that the gear is properly engaged to the rack and get the table to show the least amount of slop when you push/pull on it. This will take some mechanical know how & finesse.

You can get the pinions directly from ShopBot. Call & order them sooner than later.

-B

I have a black computer box and the motors are black/red/silver. What is the difference between the models that you are asking me about, what am I not able to do if I have the older one like you are saying?

I am working on the grease and gears right now. How do I dictate if I need new pinons?

I will attach photos when I get home.

The gears are cheap. If the gear racks are dry, you need them. Looking at your parts - you need them. When you put the new ones on, crank them on until the wrench almost bends. You'll need an 1/8" allen wrench. A large adjustable wrench will help pry it off of the shaft, like a pickle fork, if you don't have a gear puller.

You have a BT Standard machine with a 4G drive system. This uses Gecko motor drivers. This is an open loop system, meaning that if you push it too hard, it will lose steps, and position. The other model available - geared more towards production work is the Alpha model. It has encoders on the motors that self-correct if it gets out of step. It is not a 'true' closed loop system, but it has more power than the 4G (about double that of the Standard) and more power/torque on a CNC router means smoother cutting.

Your Standard is fine for what you are doing, but looking at your cuts, it needs to be tuned up. Also, the router is OK, but consider upgrading to a spindle (it doesn't bog down like the PC router) after you make some money.

-B

Quote:

---

Originally Posted by Brady Watson

The gears are cheap. If the gear racks are dry, you need them. Looking at your parts - you need them. When you put the new ones on, crank them on until the wrench almost bends. You'll need an 1/8" allen wrench. A large adjustable wrench will help pry it off of the shaft, like a pickle fork, if you don't have a gear puller.

You have a BT Standard machine with a 4G drive system. This uses Gecko motor drivers. This is an open loop system, meaning that if you push it too hard, it will lose steps, and position. The other model available - geared more towards production work is the Alpha model. It has encoders on the motors that self-correct if it gets out of step. It is not a 'true' closed loop system, but it has more power than the 4G (about double that of the Standard) and more power/torque on a CNC router means smoother cutting.

Your Standard is fine for what you are doing, but looking at your cuts, it needs to be tuned up. Also, the router is OK, but consider upgrading to a spindle (it doesn't bog down like the PC router) after you make some money.

-B

---

Thanks again. I applied grease to everything and the pinons and rack seem to be meshing well. Still trying to understand why the new gears if they are not worn and meshing correctly?

What is more important, a spindle or getting an alpha machine all together?

What do you mean the gears look dry? Are you referring to just grease? I can't find much play when the motors are powered up, MAYBE. .004. After maybe replacing gears, what else can I do? What cutters would you suggest for a good finish on either material? Feeds and speeds?

Seriously, thank you for taking some time to help me. I was also told to get nice collets from precise its.com. So those are on the way

Pinions are cheap...less than $50 for the pair. They are the only consumable on the machine besides the spoilboard. If they were run dry for even a week or two, they are shot. When they are worn they will kill your edge quality.

Hold down is a major factor in edge quality. Just screwing down a sheet in a few places is not good enough if your intent is to get top quality parts. Hold down is about 85% of the entire work involved in machining anything. Just onion skinning the parts (film left on bottom) does NOT mean that the parts cannot be pulled into the bit.

The toolpath strategy, if quality is the concern, should be made to cut the part 90% of the way with a .02" allowance, stepping down say, .1 to .2" per pass. Then come back and do a final pass cleanup @ 100% depth, stepping down the whole way with 0 allowance to shave off that .02" - nice and steady at a speed proportional to the size of the part. You are not going to get clean parts that are 3" in diameter cutting at 3 inches per second...this violates the laws of physics.

The rest of the machine should be checked with a dial indicator for slop. This is the only way to gauge what is up. The v-roller bearings can be adjusted as needed if there is slop between them and the corresponding rail.

Climb vs conventional - if the scrap is cleaner than the part - reverse the cutting direction.

Your post processor in CAD/CAM should be outputting arcs & not straight lines when cutting curved parts. Toolpath and save a simple profile toolpath around a circle. Open up the SBP. It should show about 10-20 lines of mostly CG commands. If it has hundreds of lines of code just to cut out a simple circle - you want to choose a post that commands the tool to cut with arcs - not thousands of very small straight lines to cut a circle.

There are a lot of little things that can be done to chase down quality. This is hard to do on a forum...You can have a tech come to your shop to help you with all of the things I just mentioned & give you some CNC training. You'll have to call SB about this - I have retired from doing this.

-B

I cut alot of HDPE sheet goods and can honestly say I have never gotten a "perfect" edge. You can get pretty darn close but everything shows. sometimes a quick pass with a heat gun can clean it up a little more to. another though that I didn't see mentioned - we once had a guy trying to cut round frames for something. This particular guy thought he knew better then anybody else and refused to use the Partworks software and instead wanted to make his parts using some other program and then export and import into partworks to compile the toolpath. End result was a circle that looked perfectly round on screen but when cut appeared to made of a thousand flat sides. the program he used drew circles with a **** ton of nodes as apposed to the 4 nodes per circle found in partworks. (Brady met the pint sized hipster of which I speak!). Not surewhat softare your using but I figured I would throw it out there.

Not sure if this applies, I have seen folks wave a butane torch over HDPE and it smooths everything out