Sucess now failure.

[gundog]

I cut a sheet of parts out of 1.25" UHMW they are rollers 4" round. The finished part has 4 different tool paths. The first tool path is a counter bore for a bolt head or nut 1.25" Dia .750 deep. I then flip the sheet and create a pocket in the part. Next I drill the axle hole .5" Dia. and it centers in the counter bore from the other side. Last step is the profile of the part. The first batch I made like this I got a poor finish quality for the roller edge. It was suggested to me on here to cut them oversize and make a final pass to finished dimension. The next sheet I did this I cut them .050” over size and then made a full depth cut removing the .050” and they came out with an acceptable finish I was very pleased mind you the finish was not mirror smooth but acceptable. The original profile tool path was cut with a .5” Onsrud up cut spiral bit designed for cutting this material the plunge depth was .375” and the cut speed was 1” per sec. The finish pass was full depth cut at .75” per sec. leaving a .100 - .050” skin material has some thickness variation.

I ran the exact same tool paths on the next sheet and got very unacceptable results worse than the original batch. I have been holding the material with deck screws. I tool pathed locations for the mounting screws so they would not interfere with the tools path while cutting, I used the exact method on both runs with very different results. The bad batch not only came out rough but also slightly not round.

The material size is 48x30 inches. The cost of this material is over $16 Sq Ft so I can't just through it out. Now I am forced to turn it all on a lathe to make it round and it ends up undersized which then forces me to turn a mating part to a smaller diameter this is all eating up time and losing me money.

The material had 12 screws holding it including 2 screws in the middle of the material. I should also say the parts where made with a skin and cut out of the material with a laminate trimmer. I am not sure what to try next. Experiments with this material is very costly.
Mike

This is the actual batch that went sour the picture was taken right as the last profiles where cut just before the final pass.

http://img.photobucket.com/albums/v292/millnut/DSC04712.jpg

[sawdust535]

When you say: "I ran the exact same tool paths on the next sheet and got very unacceptable results worse than the original batch" it sounds to me that something is not secure. Either the material or the tool itself.

[gundog]

I am thinking you are right but I just don't think anything moved. Looking the parts over it seems the final cleanup pass caused the problem. I saved all the tool paths separetly and I did not even shut off the machine in between the last 2 tool paths I just started the new path as the last one finished. I was so happy after the previous batch now I am not sure what to do.

I may just start making them all oversize and finishing them on the lathe but I really don't want to. It would save me so much time if I could just get it to work right. I cut these same parts over and over. I cut 2 sheets of these about once a month or two sometimes more.
Mike

[sawdust535]

Are you running the first tool path from home position, or using a 2-D Offset.

[joe]

Very Interesting. I don't like to see problems like this occure.

I seems you are doing everything correct. So it's the cleanup which is causing the problem. Your speeds are good. Should be able to run this file at 4 or 5 ips.

How did you generate the DXF?

Could you please look at your original file and see how many nodes are on the outside perfery. Should be no more than a half dozen on each part. If the router is going from node to node and there are 50 or so that could be causing the chatter.

Chatter is no stranger here. Perhaps another botter has a better answer.

Joe

[gundog]

The DXF was created with part works. For some reason I can't seem to upload my files on here. I draw all my parts on my laptop. When I try to upload them by clicking the upload button I browse for them and they are not there. I can go right to them on the computer. It must be some damn Vista thing. I have been attatching the files to my email and then opening them on the computer in the shop.

[joe]

Michael,

That's allright. How many nodes in your circle?

[srwtlc]

Michael,

Another thing to check is what Post Processor you're using when you save the tool path. Use the "ShopBot Inch Arc" PP and not the plain inch PP as it will segment your arcs with M3's.

[larry_r]

Michael

I would check to see what directon your cuts are. I often cut wood using a climb cut for the rough cut and a conventinal for the finished. Not sure what is best for UHMW. Do not be afraid to experiment with cutting directions. It can make a big difference.

Larry

[gundog]

Joe,
I am counting 8 nodes in each circle.

Scott,
That went over my head I am not sure how the Post Processor is saved how do I check that?

Larry,
I cut them in the conventional direction and not climb but I am willing to try something new.
Mike

[joe]

Michael,

Scott may be right with his suggestion. While your design program has the proper number of nodes, they may be segmented. That would cause the chatter you are having.

[gundog]

I used the circle tool in part works to create the circles. I don't know too much about drawing in cad. I am not sure if the circles are segmented or not how can I check?
Mike

[gene]

How porus is this material? could it have dulled the bit enough to make it chatter and give a rough finish ? why dont you run the file in something like mdf and see if the results are ok. this will tell you if the problem is mechanical or in software . Hope this helps some. Are you using a router or spindle ? mount may have loosened up a tad.

[srwtlc]

Micheal,

When you save the toolpath in Part Works (not the drawing), there may be more than one choice of Post Processor in the drop down list. Choose one that reads "Arcs_Inch" instead of "Inch". If you have an Alpha, choose the one for Alpha control.

I use Vcarve Pro, but Parts Works should be the same, just fewer choices.

If you just open the .sbp file in an editor, the PP should be stated in the file. If it was made with just the "inch" one, the file will have only M3 moves and no CG's. That can give you segmented move circles. Your drawing may have a cicle, but the post processor is generating code that is segmented with M3's instead of CG's.

This all assumes that your tool is tight and is not chattering from something being loose.

Scott

[joe]

Michael,

I wish I could be of further assistance but I've never owned or used Part Works but know the settings "Arch Inches is the right track.

There must be a bizzzilllion posts on chatter and rough cuts. Do yourself a favor and call SB Technical. I don't think you've done anything wrong.

[beacon14]

If the results were OK on the first run then the toolpath must be OK, something has changed between the first and second runs. The bit dulling is a possibility, especially since the first pass was just OK not great, a slight degrade in performance might be the difference between just OK and not OK. If you are putting screws into the same locations on the table could the screws could be loosening?

[bpfohler]

Is it possible when you flipped the sheet the new placement wasn't correct?
If you drilled a 1/4" hole to hold a deck screw there may be enough wiggle room to cause poor placement.
Securely fasten a ledger board to the table to help with placement when you flip the sheet.

[gundog]

I only flip the sheet after the counter bore so even if the counter bore were off it would not have caused the problem. I drilled 1/8" holes so they had no slop. I also moved the material and did not screw into the same holes. I use a laser edge finder to dial in the material so I can move it around and not screw into the same holes. The holes are slightly offset so they don't even go into the same hole when I flip the sheet. I have a 3/4" 4'x4' piece of sacrificial plywood on top of my table I screw into and I move around on it when it gets bad I plan to change it. The sacrificial piece is also screwed down countersunk below the surface by 1/4" and has probably 20 screws in it.

The bit dulling is possible but I sure hope I get more cutting out of these bits for what I paid for them $68 ea solid carbide and it probably has 10-15 hours use on it. I will check to make sure my router mount is not loose.

This is what it says were I saved the tool path.

Shopbot(arcs)(inch)(w/speed)(*.sbj

[beacon14]

Can you try it with a new bit? 10-15 hours of use in a difficult material is a lot.

Tweaking spindle speeds and feed speeds can extend bit life significantly. Vacuum hold-down might also improve quality and bit life.

[Gary Campbell]

Michael...
We have dulled bits in an hour but using conservative cuts and slow move speeds. Try slowing the spindle down, maybe tweaking up the move speed a little. We usually have the best results under 10K RPM. Heat will kill the bit before anything. Did you give your bit "the nail test"?
Gary

[gpari]

Gary Said: "Did you give your bit "the nail test"? "...

That's the one where you slam the bit into a 16d nail secretly embedded in the crappy chinese ply-board that your customer brought you, right?


I always hated the feeling of scraping off some thumb nail, gives me the shivers, but it works pretty good.

Michael, not sure on your original question, but it looks to me that some simple re-nesting of your parts could net you more parts on the same material (looks like you get 60 pcs per sheet right?) Treat them like hexagons, stagger every other row, you should be able to fit 67 pcs in the same sheet. Every little bit helps in pricey material. Plus it gives more cushion for a few messed up parts.

Gabe

[joe]

Michael,

Your post has intregued me, so I picked up some 1/2" HDPE last week for a test. I full well understand your problem, after my first attempt. Now that we've eleminated possible tool pathing problems and tool failute, it's on to other considerations.

Although HDPE isn't exactly the same molecular make up, I bleieve they show simular tool marking. For those who haven't routed this material, it cuts like a dream. The smoothest material I've ever cut. The disadvantage is, it shows every tooling flaw or chatter.

A quick test today will concentrate on bit choice and deflection. We'll see.

[dana_swift]

Michael and Joe- UHMW and HDPE are both poly-ethelyne plastic and machine identically as near as I can tell. They are both super easy to cut but do leave machining marks for me too.

Generating SBP files from CAD programs creates some very odd surface irregularities (several thousandths) which is built into the cut files from round-off errors. I don't get that chatter when I generate the SBP files from my own tool path generator. However tool marks are present in both cases.

I use a PC router and have figured that a spindle would probably hold the bit one or two thousandths "more true" at the tip of the cutter, but I have not made the upgrade (yet).

Michael, have you checked the runout of your router with a dial-indicator? If it is perfect you will still get tool marks in these plastics, but it will be minimized..

D

[joe]

Michael,

I finished a couple of tests on HDPE. The attached photo is exagerated as I Photoshoped them and increased the contrast. I real life the circle on the bottom has very, very slight tool marks. I used a Belin O #12635. It's my favorite on plex.


7524

The only difference in these was the spindle rpm. The top one was at 9000rpm while the bottom was at 15000rpms. Both cut at 1.5 ips with a 2.0 stepdown. The materials was 3/8" The bottom piece is much cleaner.

Joe

[paco]

For me there's nothing like a light finishing pass (removing a leftover allowance - 0.01-0.03) to create a very smooth edge... pretty much in all material... when required. I also have improved a lot my cuts with the spindle upgrade.

This is 1/4" aluminum.


7525

This is 1/2" HDPE.


7526


7527

[joe]

Paco,

That doesn't seem to be as affective with HDPE as other materials. Are the samples you are showing HDPE?

[paco]

Yes it is. This final pass remove most/all chatter marks from previous heavier cuts and "water marks" from multi-passes machining.

Here another view of the same part.


7528

Here Polycarbonate.


7529


7530

This last finishing pass is generally quite slower than the previous one(s).

[coolhammerman]

Occasionally I use HDPE in either 3/8" or 1/2". Although there are special "O" flute bits made for plastic, I usually just use a 1/4" two flute solid carbide cutter from Woodline USA for about $14. This is my workhorse cutter for all things sheet goods -- 3/4" BC ply to 3/4" - 1/4" cherry ply, MDF, etc.


7531

PRT 4896 2ips plunge .9ips PC router

Here are some jig pieces made that way.


7532


7533


7534


7535


7536

These didn't have to be extremely smooth so I didn't utilize a final clean up cut at a much slower feed rate. From a few inches they appear to be nice and smooth. However, when the light catches them just right if you are up real close with your good glasses on, you can easily see that they are not completely smooth. For scale, the hole is 1/4" and overall length is 4".

I could have slowed the feed rate to 1 ips or less to get a better finish. HDPE does cut like butter and is a joy to work. I also understand that it is about 5 times less expensive than UHMW. HDPE does not get gummy when machining and it is very easy on cutters. I haven't had a situation where I needed anything smoother.

As far as precision, cuts are very precise and what I consider extremely accurate. When I make parts that have to fit into another with no slop, it works just fine.

Good Luck, Ron

[joe]

Thanks Boys for the photo's. They tell much more about finishing than a million words.

HDPE is such a dream to cut. I doublt it would ever dull a bit. Like Ron says, one technique for getting a better cut is travel speed. That along with a clean up cut may be the answer.

Thanks again, I'll have to give it a try.

Joe

[gundog]

I do cut some HDPE also and it is easier to get a good finish on than UHMW regrind. I have cut a lot of HDPE with straight flute wood cutting bits with a hand router and have gotten very good finish.

For the question asked before no my bits have not had a nail test.

The pictures in Joe's post are not acceptable finish for my parts unless they are greatly magnified.

Gabe,
I agree on the re-nesting and getting more parts. I actually went the other direction to make sure I had a large frame of material left so the screw hold down will work better. When I go to vacuum I will machine closer to the edges and stager them and get more parts per sheet.

I am hoping I can get these bits sharpened so I can get more use out of them.
Mike