CNCShark HD3 Randomly digs into wood - HELP!

Discussion about the CNC Shark Pro Plus HD

Moderators: sbk, al wolford

Re: CNCShark HD3 Randomly digs into wood - HELP!

Postby xoneeleven » Tue May 09, 2017 11:38 am

Thanks Steve,
We did test slowing the pass rate down and splitting the passes into two.
The same issue occurs at the same location.

The next attempt will certainly be on the backside of the wasted boards and will try slowing it down to -100ipm

You mentioned you "had" an HD4. What do you have now?
It may be time to sell and upgrade.

Mark
Mark
CNC Shark HD3
xoneeleven
 
Posts: 33
Joined: Fri Aug 19, 2016 3:41 pm

Re: CNCShark HD3 Randomly digs into wood - HELP!

Postby SteveM » Tue May 09, 2017 12:08 pm

I returned the shark to Rockler and ordered the Axiom. It was more money, but after using it for even the short time I've had it, I feel it was money well spent.
Everything on the machine is Steel and cast aluminum. No flex anywhere on the gantry or any place else and I have actually cut at 150 and 200 ipm without any flex in any axis.
SteveM
 
Posts: 100
Joined: Thu Sep 08, 2016 1:29 pm
Location: Franklin, Wisconsin

Re: CNCShark HD3 Randomly digs into wood - HELP!

Postby xoneeleven » Tue May 09, 2017 3:42 pm

So, we ran the third sign to the final detailing toolpath of the center area of the board.

The toolpath passes are failing to lineup correctly. In addition to the other issues described previously, these issues have sprung up:
1: The first pass and second pass are not lining up. It appears to be happening on the right side of the lettering almost exclusively, and not too badly on the left side. (odd).
2: The lettering toolpath is digging slightly below the pocketing toolpaths. Note that we gently sanded the fuzzies off around the area we place the zeroing plate on, and re-zero "Z" each bit change..

Forgive me for being such a newb. I have had this machine for 11 months, and have only used it a dozen times (much more this month).

So, either I am finding problems as the result of my designs, or there is an issue with the machine, or both.

I have attached a copy of the VCarvePro design file, if anyone is interested.

final pass 3.jpg


final pass 2.jpg
Attachments
YHWH Circular Word Wrap 2x2 v3 corrected 05082017.zip
(4.99 MiB) Downloaded 12 times
Mark
CNC Shark HD3
xoneeleven
 
Posts: 33
Joined: Fri Aug 19, 2016 3:41 pm

Re: CNCShark HD3 Randomly digs into wood - HELP!

Postby Rando » Tue May 09, 2017 5:19 pm

Mark:

My calculations (using GWizard) show you're going WAY too fast on the 1/4" bit, assuming it's a 2-flute carbide endmill.

A better cut for the 1/4" bit (two flutes, right?) would be 12K RPM, 90 IPM and 30 IPPM (Plunge). At those, you're better off taking the full 0.25" depth in one pass, and with a larger step over of 0.050" (20%). That will get you a much more productive run, even though the system is running "slower".

The cutting parameters you're currently using (12K RPM, 150 IPM 50IPPM @ 0.125" DOC and 0.025", 10% SO) uses high speeds like you'd see in a very rough cut, but with a depth of cut and step over more useful for a finishing pass.

Similarly for the V-bit, speeds and feeds should be more like: 12K RPM, 36 IPM, 11 IPPM, with 0.18 DOC and 0.01/0.03 stepover. That is a finishing pass, definitely.

To a certain extent if you can up the RPM, you can move faster. But, as many of us have seen, the faster you push it, the more the system flexes.

One question is: does the V-bit have a flat on the bottom of the bit, or does it come to a nearly-zero-diameter point? In the settings for the V-bit, your notes show the overall tool diameter of 1/2", but you have 0.250 as the Diameter setting.

Another question (apologies if you've already gone over this) is how are you capturing Z0 for the bit change? If you can verify the depths that are actually being cut, that might give us a clue as to where things are going weird.

You are running the 1/4" bit FIRST, right? And the V-bit SECOND, right? Can you give us a photo after the 1/4" has finished, but before you've run the v-bit? That might help figure out what's going on.

What is the role of the "YHVH climb" toolpath? Are you running that in these tests? Also, I'm not clear on why there is both a V-Carve and Pocket for the outside ring. But, let's solve the inner-field issue first. I did not validate the parameters for the outside-ring cuts, but the shredding of the wood would indicate there are similar speed issues there.

One step forward.... :D

Regards,

Thom
=====================================================
ThomR.com Creative tools and photographic art
A proud member of the Pacific Northwest CNC Club (now on Facebook)
Rando
 
Posts: 396
Joined: Tue Jan 06, 2015 3:24 pm
Location: Seattle, WA

Re: CNCShark HD3 Randomly digs into wood - HELP!

Postby SteveM » Tue May 09, 2017 5:30 pm

Looking at the tool paths, I see your second and third cut you have a .25 60 degree bit at the top and a .25 end mill for large area clearance tool..
Please correct me if I am wrong, but wouldn't you just use the .25 end mill for clearing out the larger waste and just have 1 tool path without the V-bit.
I am no expert, but I don't think that looks correct.

I would post that file at the Vectric forum where there are some really sharp people that can help you out.
SteveM
 
Posts: 100
Joined: Thu Sep 08, 2016 1:29 pm
Location: Franklin, Wisconsin

Re: CNCShark HD3 Randomly digs into wood - HELP!

Postby xoneeleven » Tue May 09, 2017 10:59 pm

Thanks Thom and Steve,
I believe your assertions regarding the speeds and stepover are correct.
Those feeds and speeds were taken from someone I talked to that has a much more robust machine that I have, and I am betting he recommended those based on his setup, and not mine.

As far as the extra tool paths. Those were put in to try to figure out the initial problems I ran into. They have since been removed.

I also learned to keep the stepover to as close to "0.0" as possible on vbit finish passes.

I have been running the clearance cut and then the vbit cuts (in that order).

We went ahead and finished cutting out the edge lettering, but ran into similar issues where the final toolpath using a tapered ball nose bit cut deeper than the clearance toolpath. (like you saw on the other photos with the larger areas)

As far as checking the bed flatness, I have a spoilboard that I flattened using an end mill. I would expect the bed to be very flat, still. It is in pristine shape. However, I will certainly check it with a straight edge tomorrow.

I really do appreciate the advice, gentlemen.
Mark
CNC Shark HD3
xoneeleven
 
Posts: 33
Joined: Fri Aug 19, 2016 3:41 pm

Re: CNCShark HD3 Randomly digs into wood - HELP!

Postby Rando » Wed May 10, 2017 12:21 am

xoneeleven wrote:
As far as checking the bed flatness, I have a spoilboard that I flattened using an end mill. I would expect the bed to be very flat, still. It is in pristine shape. However, I will certainly check it with a straight edge tomorrow.

I really do appreciate the advice, gentlemen.


Glad to help, hope progress is made.

That makes sense with the F&S being fast; you do have to be a little cautious with the sharks because of the HDPE elements. However, as you become more familiar, you'll come to realize that feeds and speeds are not nearly as much about machine rigidity as they are about the bit in the material. So, if your friend is cutting using those parameters in the same material, then they are also doing it wrong. That is especially true of that 0.125" DOC 10% SO cut: it's moving way too fast at that spindle speed to cut the wood properly. It's all about the chipload, and that has a wicked high chip load, and that's what leading to the shredding. Wood has a wider sweet-spot for the cut parameters, but that does not mean the params can just be chosen willy-nilly. Good cuts are ones that remove the material quickly, with the necessary finish quality, within the limits of the machine. Spinning or moving a bit too fast OR too slowly will cause the bit to dull more quickly than when used properly, and it will produce lower-quality cuts, with burrs and all that.

E.g,. I have a 3/16 and 1/4" endmill I've been using for over a month in many different projects over the last two months, and they're still going strong. Why? Because I've tuned those F&S so they are optimal for the bit and material, while working within the machine's capabilities for making the cuts accurate, and not letting it "get into trouble" because of the lack of rigidity. The thing is, when it's all said and done, your 1/4" end mill and your wood are the same as his 1/4" end mill, so getting high-quality accurate cuts is still going to want the same parameters.

The other day, I got a sample part from my local endmill supplier (they manufacture their own line of endmills) where they did some amazing cuts on a $250K machine...and it had chatter, and bad pocket-bottom flatness, and all the things I used to see on my machine, and in some ways, I get better results than they did. Yes, they ran it faster and deeper, but the cutting geometry was the same, and the effects of deflection and chatter were present on their part too.

For the spoilboard and ruler, I was actually talking about the stock material warping, and lifting itself up from the spoilboard, but in the middle. So, the straightedge should be applied to the backside of the wood you're carving, not to the spoilboard's leveled surface.

Can you describe what effect you're going for, using the tapered ball mill after the v-bit in the YHVH toolpath? Usually that V-bit cut would be the end of it, since it is the finishing pass to the 0.250" endmill's clearance (aka roughing, or hogging) pass.

Well, tomorrow will shed more light on the subject. Good luck :D.

Regards,

Thom
=====================================================
ThomR.com Creative tools and photographic art
A proud member of the Pacific Northwest CNC Club (now on Facebook)
Rando
 
Posts: 396
Joined: Tue Jan 06, 2015 3:24 pm
Location: Seattle, WA

Re: CNCShark HD3 Randomly digs into wood - HELP!

Postby sharkcutup » Wed May 10, 2017 5:32 am

I know that this may be a bit late!

Why have you not tested/tried out your tool paths on a smaller scale on a cheaper wood type first? Or even the same wood type but on a smaller scale first? I know that there will be a change in feed/speed rates in the different woods but at least you would have proven out your tool paths (order, depths, finish looks, etc...). If I am unfamiliar with a particular tool path, router bit, etc... I usually test out my tool path on a small scale on cheap pine, poplar, etc... first, then after I am satisfied with the results I upgrade to the wood type for the finished product and adjust accordingly on the rpms and feed/speeds. I also know that all the testing/try outs are time consuming but in the long run I not only have learned from it but I have a product that I am satisfied with in the end!!!

Another thing you might want to remember and/or consider is that if you should happen to get the router bit to hot (running too fast or too slow) you could very well change its temper strength and sharpness thereby ruining a perfectly good bit. That in itself can be costly replacing too!!! I have actually seen this happen to a perfectly good 1/4" end mill.

Sharing some knowledge/experiences from my CNC cookbook (anyone care to try some of my hot 1/4 end mills, hehe :lol: )

Good luck in solving your issues!!! ;)

Have a GREAT DAY!!! :D

Be SAFE around those AWESOME machines!!! ;)

Sharkcutup
sharkcutup
 
Posts: 255
Joined: Tue Mar 08, 2016 5:23 pm

Re: CNCShark HD3 Randomly digs into wood - HELP!

Postby xoneeleven » Wed May 10, 2017 8:13 am

All of you guys have great insight and advise.

Thanks for the insight sharkcutup, Steve & Thom and Bob !
Mark
CNC Shark HD3
xoneeleven
 
Posts: 33
Joined: Fri Aug 19, 2016 3:41 pm

Re: CNCShark HD3 Randomly digs into wood - HELP!

Postby xoneeleven » Wed May 10, 2017 8:21 am

Rando wrote:
xoneeleven wrote:
Can you describe what effect you're going for, using the tapered ball mill after the v-bit in the YHVH toolpath? Usually that V-bit cut would be the end of it, since it is the finishing pass to the 0.250" endmill's clearance (aka roughing, or hogging) pass.

Thom




I was wanting to have it extremely smooth between the lettering inside that ring.

Unfortunately, the same thing happened in that area. The end mill toolpath was fine, but the finishing toolpaths cut too deep.
Mark
CNC Shark HD3
xoneeleven
 
Posts: 33
Joined: Fri Aug 19, 2016 3:41 pm

PreviousNext

Return to CNC Shark Pro Plus HD

Who is online

Users browsing this forum: No registered users and 2 guests