Text-On-Text Issues

This forum is for general discussion about Aspire

Text-On-Text Issues

Postby TimSchubach » Sun Jul 02, 2017 3:13 am

I've had a Shark HD for about 5 years, and have had few problems with it, other than the connecting rod from one of the servo motors loosening from the screw rod and destroying a nice piece of wood. One thing I've been trying to do recently is a simple text-on-text project using Aspire v8.5. I've been at a new job for about 7 months, and I still don't have a name plate so I thought I'd make one myself. Fast-forward four name plates later, I still don't have one I'd want to display in public.

I use four different tool paths: one each for clearing the top and bottom layers ( 3/16" end mill ); one each for detailing the top and bottom layers ( 1/16" end mill ). I first combined the two sets of common tool paths, and cut two tool paths. What happened was that the detail tool path always cuts deeper than the clearance tool paths on both layers. It's very noticeable, and it looks bad. A friend of mine has access to an Axiom machine, and he had me convinced that there was too much play in my machine ( I cannot argue that there IS some play in the assembly that holds the router ), so he volunteered to generate gcode for the Axiom and run it on that machine. He does not have access to Aspire, so I saved my project in VCarve Pro format. We were both pretty confident that the result would be different, and I was already looking into prices before he even started to cut my project. Three days later when he had time to finish the project, we saw the exact same results. So I know the issue is not my machine.

I've tried cutting the project several different ways: all of the top layer first, then all of the bottom layer; clearance on top and bottom followed by detail top and bottom; detail first ( presumably to minimize chipping from the clearance bit ) followed by clearance; reset virtual zero between all tool paths; just reset Z0 between tool paths ... I'm getting the same result. I've also cut projects out of both Oak and Walnut. The only thing I want to try, but have not because I can't figure it out even after watching the Vectric tutorials, is rest machining. Since this is not 3D, I wouldn't expect to see a difference, but I've been wrong too many times to count already.

While my clearance bit has been used a few times prior to this run, the detail bit was brand new.

Fortunately, I don't have any paying customers waiting for me to figure this out, but I'd sure like to be able to show my customers what I can do. Until I can figure this out, I'm not even mentioning it to any of my customers.

I've attached a picture of part of the last finished project from the Axiom machine, as well as the VCarve Pro version of my project ( tool paths deleted due to size restrictions for posts ). If anyone sees anything obviously wrong, or has any suggestions, I would be most appreciative.

Tim
Attachments
WDN_1758[2].jpg
Name Plate.crv
(59.5 KiB) Downloaded 28 times
TimSchubach
Vectric Apprentice
 
Posts: 51
Joined: Tue Mar 19, 2013 4:41 am
Location: Miamisburg, Ohio
Model of CNC Machine: CNC Shark HD MAKO

Re: Text-On-Text Issues

Postby highpockets » Sun Jul 02, 2017 3:53 am

Your attached .crv file doesn't have any toolpaths so it's hard to say. If your machine and your friend's are cutting the same then I'd rule out in proper Z zero setting for the finishing tool. If the preview shows no issues then it is more than likely a machine setup issue.
It would help a lot to see the .crv with toolpaths.
John
Maker of Chips
User avatar
highpockets
Vectric Wizard
 
Posts: 1286
Joined: Tue Jan 06, 2015 4:04 pm
Model of CNC Machine: PDJ Pilot Pro

Re: Text-On-Text Issues

Postby TimSchubach » Sun Jul 02, 2017 5:45 am

Hi John - Yes, of course ... the file was too large to post with the tool paths, and I was focused on reducing it's size. The fact that the file was worthless without the tool paths didn't sink in.

OK, so the file is still too large to post with the tool paths, so I uploaded it to a read-only OneDrive folder https://1drv.ms/u/s!Ai2G_TPTNBp3sGsYFQ99iYn8gGs3. The Top Layer has a Start Depth of 0.0" with a Cut Depth of 0.18", and the Bottom Layer has a Start Depth of 0.18" with a Cut Depth of 0.18". And the preview does not show any issues.

If this is a machine setup issue, I'm at a loss as to what it is since the two machines have different setups.

Thanks,
Tim
TimSchubach
Vectric Apprentice
 
Posts: 51
Joined: Tue Mar 19, 2013 4:41 am
Location: Miamisburg, Ohio
Model of CNC Machine: CNC Shark HD MAKO

Re: Text-On-Text Issues

Postby highpockets » Sun Jul 02, 2017 6:22 am

Tim,

I looked at the crv file. All looks good there and the preview is correct.

Lets forget about your friends machine, that's just complicating things.

How are you setting Z zero on your machine?

Are you running the two clearing toolpaths then changing bits and running the two finish toolpaths?
John
Maker of Chips
User avatar
highpockets
Vectric Wizard
 
Posts: 1286
Joined: Tue Jan 06, 2015 4:04 pm
Model of CNC Machine: PDJ Pilot Pro

Re: Text-On-Text Issues

Postby TimSchubach » Sun Jul 02, 2017 7:00 pm

Hi John,

I've run the file three different ways: first by running the two clearance tool paths ( output as one combined .tap file from Aspire ), and then the two detail tool paths ( also one combined .tap file ); running the detail paths first and then the clearance; and running everything on Layer One ( two tool paths ) first followed by Layer Two ( two more tool paths ).

Initially, I used my touchpad and ran the virtual setup before running the clearance path, and then used the same Virtual Zero settings for the detail path - just had to detect the touchpad after the bit was changed to get a new Z0. I've also rerun virtual set when I changed the bit, just in case there was any movement in the piece due to wood having been removed. I have to believe that changing the bit and finding Z0 a second time is my issue, but I don't understand how/why.

I kind of jokingly told my friend that I could probably solve this issue by using the 1/16" bit for the whole thing ... if I didn't mind waiting a week for the tool paths to cut.

One other thing I suppose I could try is to make this a 3D project - I think I'd just have to pick a different font since there are some "thin" areas on some of the letters. At least that should eliminate the problem, bit would take a LONG time to cut.

Not that I think this has anything to do with it, but I do run my bits kind of slow, or so I've been told. I think I run the 1/16" bit at 30 in/min at 1/16" pass depth, and the 3/16" at 50 in/min at 1/8" pass depth. I guess I'd rather sacrifice on time over broken or burned bits.

Thanks,
Tim
TimSchubach
Vectric Apprentice
 
Posts: 51
Joined: Tue Mar 19, 2013 4:41 am
Location: Miamisburg, Ohio
Model of CNC Machine: CNC Shark HD MAKO

Re: Text-On-Text Issues

Postby TReischl » Sun Jul 02, 2017 7:23 pm

Tim, I think you might be right about having a problem getting Z zero correctly when changing bits. It is either that, or your wood is really bowing after the roughing cut. Which I highly doubt since it appears pretty even across the pic you posted.

I am going to introduce another concept to you and do not take it the wrong way.

The Sharks are not known for their rigidity.

If'n it were me I would do the following:

Rough mill the pocket leaving about .010 -.015 on the bottom. I would then do a finish cut with the same tool at full depth. That should remove any issue of the tool flexing upwards as you are cutting.

Then I would run the small tool. Look to see if it was flush with the tool used to remove most of the material. Hopefully it is.

What I am trying to tell you is that sometimes you have to make finish cuts, not just select "Pocket" and set the final depth. The other projects you have been doing for the last five years may not have revealed any flex in your machine, especially at the feedrates you use. You should do yourself a favor and try double those feeds. I am not a big fan of Sharks, but the machine should be able to handle it. I believe 4D runs one? Could be wrong, maybe he can chime in here and give you some ideas on feeds.
http://www.tedreischl.com

Low Profile CNC Router Vise
User avatar
TReischl
Vectric Wizard
 
Posts: 1966
Joined: Thu Jan 18, 2007 6:04 pm
Location: Leland NC
Model of CNC Machine: 8020 Build 48X36X8 RP 2010 Screenset

Re: Text-On-Text Issues

Postby highpockets » Sun Jul 02, 2017 8:31 pm

I'm running out of suggestion hear, hopefully someone can step in and solve this issue.

I still believe it's a Z setup issue.

Here is one last suggestion, go back to old school, by that I mean don't use virtual zero (it shouldn't be an issue with the problem, but taking everything non essential out of the mix to get back to basics). Next don't use the touch plate, use a piece of paper or feeler gauge to set Z zero manually. This problem with a conductive touch plate is you are relying on the conductivity of the bit.
One other thought to get your name plate made. Run a bottom (clear) with your 5/16" bit then a second bottom (clear) with your 1/16" bit. Since your finish bit has been running deep it won't matter.
John
Maker of Chips
User avatar
highpockets
Vectric Wizard
 
Posts: 1286
Joined: Tue Jan 06, 2015 4:04 pm
Model of CNC Machine: PDJ Pilot Pro

Re: Text-On-Text Issues

Postby Mobius » Mon Jul 03, 2017 3:24 am

This is a problem I often fight with. I've found it can be a combination of things that can result in this effect, and I also find that I forget one or more of them more often than not. This results in furious sanding and chisel touch ups. You will likely have to set up a test piece and keep trying different things until you solve the problem.

1. Zeroing. If the effect is consistent throughout the whole piece, this is the first thing I would look at. As mentioned try zeroing manually.

2. Tool offsets. I'm not familiar with the Shark and what they use for control software, but do some searching around and make sure no tool offsets have been accidentally applied to that tool number. This would consistently ruin your zero.

3. Tool type. Are you using the same type of end mill for both operations (ie: flat bottom end mills, or fishtail bottom end mills, or single flute spirals etc.) They all cut a bit differently, and can leave a different bottom finish which would then be visible.

4. Relating to #3 is feeds and speeds and cut depth. If you're hogging out a bunch of material in each pass with the larger bit, the slight deflection caused by this stress will cause the bit to be slightly shorter. Which means the cut won't be as deep as your finishing path. As mentioned, you can set up your bottom pass to take a minimal amount of material, reducing the stress on the bit. You may have to play around with cut depth, feedrate and stepover to find an optimal bottom finish.

5. Relating to #3 and #4 is tool length. Again, deflection is your enemy. Use the shortest bit possible for each operation.

6. Material hold down and material thickness. How is your material clamped to the spoilboard? Screwed down? Clamped on the edges? Vacuum table? I've found that when I clamp my material on the edges, it causes it to bow up slightly in the middle. I've resorted to using carpet tape underneath the material to keep it stuck securely to the spoilboard, with clamps on the side to take the majority of the force. Even a slight bow can lead to vibration as the bit passes over the material, wreaking all kinds of havoc on the bottom finish. Thinner materials (<3/4") suffer more from this I find.

7. Time between cuts. This can sometimes come into play if you stop the cutting operations and resume them at a later time/date. Changes in temperature and humidity can cause quite a bit of movement in the wood. Even if you cut in a temperature and humidity controlled environment, the act of cutting into the wood can expose the inner wood with a differing moisture content. As the cut wood dries, it will shrink/bend/warp.

Those are some of the issues I've come across. I'm sure there are more, but they're escaping me at the moment.
Connor Bredin
Distinctive Dimensional Concepts Ltd.
www.distinctive-concepts.ca
Mobius
Vectric Craftsman
 
Posts: 253
Joined: Wed Jul 09, 2014 1:19 am
Location: Drumheller, Alberta, Canada
Model of CNC Machine: CRP Pro 4848 Custom Build

Re: Text-On-Text Issues

Postby TimSchubach » Mon Jul 03, 2017 4:42 am

I hear a lot of good suggestions that I will try, and hopefully one of them will work.

When I bought my Shark, I thought I was buying a top-quality machine -- apparently that's not really the case, which is why I was so sure the results from the Axiom would be so much better. if you haven't seen one, there is NO flex. The cutter runs side-to-side on the gantry on a pair of dovetailed splines that keep the cutter from bouncing. The fact that the Axiom gave me the same results tells me that machine flex is not the issue. And even tho the gcode is different between the Shark and the Axiom, I could be looking at an issue with how the gcode is generated ( i.e. a software problem ).

To highpocket's point, I'm not exactly sure how the Axiom sets Z0, but you can use a "touch off puck" similar to the Shark's touchpad. However, unlike the Shark, I don't think the puck is placed on the wood. I think it's placed somewhere else on the table. My friend talked about a "table origin" versus a "project origin". One of my thoughts was that if there any fuzz under my touchpad when I changed bits, that would throw off Z0. But it would cause the second cut, the detail cut, to cut more shallow, not deeper. So I scratched that as a root cause.

TReischl: are you suggesting that I only make that finish cut with the clearance tool, and make the detail cut normally?

Mobius: Point #2: again, since I got the same results on both the Shark and the Axiom, I'm not sure it this is applicable. It certainly could be, but I don't see how. And it doesn't mean I won't look into it anyway.
Point #3: No, they are not the same type of tool. My 3/16" clearance bit it is an up-cut spiral bit, but my very first attempt was with a straight, two-fluted bit. Something else to consider ...
Point #4: One of the reasons I take it a little slower and don't hog out too much at a time is to prevent exactly what you're describing. With the 3/16" bit I'm using a cut depth of 1/8", which that bit should be able to handle easily. With the 1/16" bit, I only take 1/16" at a time.
Point #6: I use four clamps on the corners to hold everything down. If this only happened with cuts in the middle, I'd think I'd need to use some double-sided tape just for insurance. But this piece is only 4" tall. As for thickness, the last piece was 3/4".
Point #7: I go from one cut to the next ASAP. Only once did I go more than about 30m, and that was because the first cut didn't finish until about 03:00.

Many things to try. Again, thanks for all your input. What I think would be at least a little telling is if someone else tried to cut that project as-is, and if they saw the same thing.

Tim
TimSchubach
Vectric Apprentice
 
Posts: 51
Joined: Tue Mar 19, 2013 4:41 am
Location: Miamisburg, Ohio
Model of CNC Machine: CNC Shark HD MAKO

Re: Text-On-Text Issues

Postby highpockets » Mon Jul 03, 2017 5:29 am

Tim,

I haven't run the job on my machine, may do that tomorrow, but I did gen the gcode for my machine. I took a look at both the clearance and finish gcode files.
Both show a max Z of Z-0.3600.

That tells me it's a machine or machine setup issue and not a VCP or PP issue. At lease not my PP.
John
Maker of Chips
User avatar
highpockets
Vectric Wizard
 
Posts: 1286
Joined: Tue Jan 06, 2015 4:04 pm
Model of CNC Machine: PDJ Pilot Pro

Re: Text-On-Text Issues

Postby TReischl » Mon Jul 03, 2017 3:21 pm

It is highly, HIGHLY, doubtful that it is a g code problem.

Every now and then I post the following:

There are thousands and thousands of Aspire users. They are creating hundreds of programs everyday. If there were a g-code issue you would be reading about it all over the board here. There are lots of Shark users out there too. They did not ship you the only version of software that does what you are seeing.

That is something to keep in mind because quite often people who are not able to read g code always have this naggy little suspicion in the back of their minds that it might be the thing they do not understand, the software. Rarely is that the case.

I stated in my other post that the Shark is not known for being a rigid machine. That does not mean you cannot get good cuts with it, only that you have to do things that do not allow the machine to ruin workpieces.

In fact, the rigidity of the machine might not be a factor at all. After all, you are running at a really, really slow feed rate.

You mention that you place the touch off plate on the work. I do exactly the same thing on my machine. I am very careful to make sure I put it in about the same place on the workpiece for all touch offs. And yup, I make sure there is no fuzz or chips in the area. The machine has the ability to then use an off piece touch off plate for all subsequent tools to set the offsets. I rarely use it since I have not had problems with touching off on the surface of the material.

BTW, usually when software screws up, it REALLY screws up, it does not alter something by a few thousandths, it goes crazy.

Since you cannot read the gcode and since you are running really slow, one thing you COULD do very easily is pay attention to the DRO on your computer screen. When the tool is at the bottom of the pocket it should read exactly the depth you programmed it to with Aspire. Check both the roughing and finishing tools. You do not need material in the machine, you can dry run to do this. If the machine is flexing, it would not change the DRO so there is no point in running a piece. By doing that, you can reassure yourself that you have told the machine the correct depth in both cuts and that the software is telling the machine the correct depth. Pretty easy to do, just sit there and watch it.

If the machine IS showing the correct depth on both tools, you are going to have to start looking at how you are setting up when you start the job and/or look at the machine carefully. I am pretty sure you are going to find out that it is a set up problem, something you are doing on both the Axiom and the Shark. But hey, every now and then I am wrong.
http://www.tedreischl.com

Low Profile CNC Router Vise
User avatar
TReischl
Vectric Wizard
 
Posts: 1966
Joined: Thu Jan 18, 2007 6:04 pm
Location: Leland NC
Model of CNC Machine: 8020 Build 48X36X8 RP 2010 Screenset

Re: Text-On-Text Issues

Postby Mobius » Mon Jul 03, 2017 3:37 pm

What about the material itself? Have you tried a different material, say (uugh) MDF? Something that is maybe a little more stable and consistent internally?

Perhaps this is still a material movement issue, and the wood is moving/swelling after it has been roughed out due to the internal stresses of the wood?
Connor Bredin
Distinctive Dimensional Concepts Ltd.
www.distinctive-concepts.ca
Mobius
Vectric Craftsman
 
Posts: 253
Joined: Wed Jul 09, 2014 1:19 am
Location: Drumheller, Alberta, Canada
Model of CNC Machine: CRP Pro 4848 Custom Build

Re: Text-On-Text Issues

Postby redwood » Mon Jul 03, 2017 9:02 pm

On the Axiom, you place the zero puck wherever you tell the software it's going to be. Usually on the surface of the material. When I've had these issues, it's usually when I have to move the puck to a different area because I've machined out the previous position. It's pretty critical that the puck be in the same position for each tool change, if those depths are going to interact with each other.
redwood
Vectric Craftsman
 
Posts: 149
Joined: Wed Apr 13, 2016 3:38 am
Location: No. Calif.
Model of CNC Machine: Axiom Pro6

Re: Text-On-Text Issues

Postby TimSchubach » Tue Jul 04, 2017 4:19 am

Hi Mobius,

No I haven't tried another material such as MDF - just Oak and Walnut. But again, that's something to try just to see what happens.

The stress question is certainly something that's crossed my mind. But if I cut the details tool path first, I would expect that not to relieve much, if any, tension. I would expect that potential "release" to come with the clearance cut, and I would expect the wood to flex up ( convex ) not down ( concave ), which would mean that the clearance cut would look deeper than the detail which is not what I'm seeing.

Hi TReischl,

You are right - I don't understand all of the GCode, but most of it seems pretty straightforward. And I would also agree that if there were a problem with Aspire or VCarve Pro, there would be a lot of chatter here.

I haven't looked at the GCode for this project yet, but just as a first-step sanity check, I did hover over the four tool paths and I see that the max carving depth is what I expect: 0.18" for the top layer, and 0.36" for the bottom layer. Whether what's reported syncs up with reality is where the issue lies.

Tim
TimSchubach
Vectric Apprentice
 
Posts: 51
Joined: Tue Mar 19, 2013 4:41 am
Location: Miamisburg, Ohio
Model of CNC Machine: CNC Shark HD MAKO

Re: Text-On-Text Issues

Postby TReischl » Tue Jul 04, 2017 7:47 pm

This idea of " Whether what's reported syncs up with reality is where the issue lies."
is where you are running into problems. It is time you found out what is really going on. The way to do that is pretty darn obvious:

You programmed the depths you want, now all you have to do is look at the gcode to see if there are any moves that are deeper than what you specified.

Open the gcode file in a text editor like Notepad. Tell it to search for all the Z- moves. Then read what it is saying. If you find Z- moves that are greater than what you spec'd you have a software problem. If not, you have a machine or setup problem.

Constantly thinking it might be a software issue is wasting your time and everyone who is trying to help you. If you cannot read the code, post it here and we can read it. Tell us what your final depth for that pocket is supposed to be and we can tell you if the code is wrong. Sitting around wondering "well, did it actually tell the machine to go to that depth" is a waste of time. The gcode will eliminate one possibility. Then we can move on to what is really going on instead of playing "what if" for post after post.
http://www.tedreischl.com

Low Profile CNC Router Vise
User avatar
TReischl
Vectric Wizard
 
Posts: 1966
Joined: Thu Jan 18, 2007 6:04 pm
Location: Leland NC
Model of CNC Machine: 8020 Build 48X36X8 RP 2010 Screenset

Next

Return to Aspire - General

Who is online

Users browsing this forum: IslaWW, Yahoo [Bot] and 22 guests