Router Forums banner

1 - 18 of 18 Posts

·
Registered
Joined
·
21 Posts
Discussion Starter #1
I have been having an issue with some simple text. All seems well in the Vcarve file, but when I go to cut the text it gets progressively deeper. Cut starts at the prescribed depth (.06) and when its done depth has gone to (.11). I am using a 30 degree vbit for this cut... seems as if the Z axis is having trouble holding its own during this cut. 7 lines, about 140 letters, so there is a lot of up and down on the z axis.... In the same file I have two pocket cuts with a 1/4" end mill that run in opposing directions to get a smooth surface, Z axis holds very well during this cut. Any suggestions?

Probotix Meteor
V Carve Pro
 

·
Registered
Joined
·
4,352 Posts
Sounds like the spoilboard needs skimming. Your work isn't level. Also, your material may not be a uniform thickness. I really have to watch when I do text on a non-machined surface.

HJ
 
  • Like
Reactions: artman60 and MEBCWD

·
Registered
Joined
·
349 Posts
I agree with HonestJohn, it would be either the bed or your material.

One sawmill that I get wood at is planed and over the 12" width it can be 0.008" different in thickness. When I v-cut some text to 0.0625" (1/16") it makes a visible difference. Especially if I used the high side for setting Z.

The tooling Z depth is relative to the gantry, so the end mill cutting flat is expected. I'm sure if you could accurately measure the pocketing to the surface that it is also off 0.05" in the same areas as the V-Carve, just not visually apparent.

My standard "fix" is in two steps. First I use a micrometer to measure the wood stock and scribble the thickness in each corner, then scribble the delta difference to the highest reading. Second I use plastic shims from McMaster Carr to raise the "low" side. I've found that the 0.005" let me get close enough that there is no visual clue.
https://www.mcmaster.com/#standard-shims/=150t1j7

To me, surfacing each piece of material is too time consuming.

Steve.
 

·
Registered
Joined
·
4,352 Posts
To me, surfacing each piece of material is too time consuming. Quote Steve

You got that right, Steve. I just keep a deck of old playing cards around and use them as shims as well as for retouching off the z axis after a bit change.

I should really get a z puck - scared of how hard it would be to set up.

HJ
 
  • Like
Reactions: artman60

·
Registered
Joined
·
3,727 Posts
Craig,

Since the cut is deeper at the end of running your toolpath I agree with John and Steve about the thickness of the material and possibly the level of the bed/spoil board to the gantry. If it was deep at the start and shallow at the end it might be the bit slipping in the collet if your material had an even thickness and the bed/spoil board is level to the gantry.

First I would check to make sure the bed is as close to level to the gantry as possible without nit-picking, then trim the spoil board level to the gantry with a large bit. This should take care of any problem with the bed or spoil board. This should also be done as part of a periodic maintenance schedule for checking bolts, alignment check and lubrication.

Then get a good caliper and always measure your material so you know what to expect when you use the material without machining it. If it will be a problem then machine the material before use or as Steve points out you might get by using shims to level the material to the gantry before machining.
 

·
Registered
Joined
·
1,171 Posts
One last thing to check is that your bits are tight in the router.spindle collet. I've stopped counting the times when a student-installed bit comes loose while cutting both on our CNCs and in conventional table-mounted routers. Upcut and straight fluted bits work themselves out when loose.

The MDF surface that probotix provides can sag in the middle under its own weight.

4D
 

·
Registered
Joined
·
21 Posts
Discussion Starter #7
The bed was leveled 3 months back, I checked the mounted material with a micrometer between the surface and the collet nut and it was within .002 on all corners. Project is 10" square... material was planed to .743 to .744 across all corners
In the pic the cut begins with the "THE THINGS" line and it left the vertical line on the T in THINGS un cut...proceeded in a counter clockwise direction. After carving about half of the top two lines it came down and picked up the I in I CANNOT, and the the vertical part of the T.. this is where I noticed the difference starting to appear. Cut goes back towards the top, worked lines 2, 3, 4, 5, 6 on the left half, returned to top to the word GOD, and then the bottom line last, which is the deepest point... the center large letters are a different cut, same tool, and it goes deeper than it should, still seems to follow the pattern of Z axis dropping? All appears to be a bit random in location for the increasing depth from start to finish. I will check the table and gantry for levels, but the results seem to show that the Z cut is getting progressively deeper thru the cut as opposed to a problem with the bed or the material.
I checked the Z screw and it really moves easily by hand going down, but you can realize the weight of the spindle when you try to turn it by hand. I did get a bit of tightening on the coupler screws, about 1/8 turn maybe.. I am wondering if the issue may be related to a mechanical problem.
I have made a few of these round medallions before, this one the content was changed but not the text in question. Previously this issue wasn't there.
I make these for a friend who works at the VA and he has request's for at least a dozen more, sure need to figure this out, thanks for listening...
 

Attachments

·
Registered
Joined
·
1,171 Posts
Any chance you can post the text/drawing file? I did a job/favor for a friend awhile back and the text she provided was a photo of text she took off a burial stone. As her aim was not straight on the text when converted to vectors varied in size from side to side. If cut as it was it would have been deeper as each letter got larger. I use the distort tool in VCarve to unwarp the text so it all looked and cut like it was a simple windows font.

Increasing depth could be g-code commanded, a Z stepper that is slipping, a bit slipping out, etc. Are the Z levels that show (in LinuxCNC) while cutting getting larger on the deeper text? Does the bit return to the height it started at when the job is done cutting? If you issue G0Z0 at the beginning and again in the same spot after cutting to see if the whole Z axis has crept down. There is a coupler between the Z motor and the feed screw. If either side of that coupler is loose it would explain your increasing Z depth.

4D
 

·
Registered
Joined
·
3,727 Posts
One more problem that comes up now and then is the movement within the wood. When the wood is cut it will release tension that is built up with in the wood and the wood actually moves. Humidity can also cause newly cut wood to distort as it draws in moisture or releases moisture. I have been having this happen lately but I am looking for it to happen when ever the humidity is high or I am removing a large amount of waste material. If this is the problem you can remove the board after roughing and let the movement settle down before doing the finish and text toolpaths.

The toolpath also jumping around does not help because if the wood is moving then it might move to a new location long enough for the wood to move then go back to the old location and start cutting at the right depth but the cut is deeper because the wood has swelled or domed. One way to help over come this is to select the text by rows or even by word or letter so it will not jump around so much. Remember when selecting vectors like this to use the "Vector Selection Order" in your toolpath "Order" tab or the "Use Vector Selection Order" in the other toolpaths that don't have the "Order" tab.
 

·
Registered
Joined
·
21 Posts
Discussion Starter #10
Any chance you can post the text/drawing file? I did a job/favor for a friend awhile back and the text she provided was a photo of text she took off a burial stone. As her aim was not straight on the text when converted to vectors varied in size from side to side. If cut as it was it would have been deeper as each letter got larger. I use the distort tool in VCarve to unwarp the text so it all looked and cut like it was a simple windows font.

Increasing depth could be g-code commanded, a Z stepper that is slipping, a bit slipping out, etc. Are the Z levels that show (in LinuxCNC) while cutting getting larger on the deeper text? Does the bit return to the height it started at when the job is done cutting? If you issue G0Z0 at the beginning and again in the same spot after cutting to see if the whole Z axis has crept down. There is a coupler between the Z motor and the feed screw. If either side of that coupler is loose it would explain your increasing Z depth.

4D
All of the file was drawn in Vcarve pro... text used was Single Line - Norm West 1L for all except the big letters in the center which I used Vcarve tools for...
I did look at the coupler and I could get an 1/8 turn to tighten both sides of it. I loosened it, then reset it as tight as I could without stripping something. A while back I had 2 of the 4 bolts that hold the spindle mount onto the gantry get loose, in fixing that I marked the spindle and mounts in a way I could tell if something moved. Also made and used a tramming tool at that time.
I don't know how to read the Z levels in the file .. I assume I can scroll thru it and see this? What am I looking for?
Bit returns to insert the next tool position, so I can check there when I mount the bit and when it returns....

Thanks for the helpful suggestions
 

·
Registered
Joined
·
21 Posts
Discussion Starter #11
One more problem that comes up now and then is the movement within the wood. When the wood is cut it will release tension that is built up with in the wood and the wood actually moves. Humidity can also cause newly cut wood to distort as it draws in moisture or releases moisture. I have been having this happen lately but I am looking for it to happen when ever the humidity is high or I am removing a large amount of waste material. If this is the problem you can remove the board after roughing and let the movement settle down before doing the finish and text toolpaths.

The toolpath also jumping around does not help because if the wood is moving then it might move to a new location long enough for the wood to move then go back to the old location and start cutting at the right depth but the cut is deeper because the wood has swelled or domed. One way to help over come this is to select the text by rows or even by word or letter so it will not jump around so much. Remember when selecting vectors like this to use the "Vector Selection Order" in your toolpath "Order" tab or the "Use Vector Selection Order" in the other toolpaths that don't have the "Order" tab.
After two attempts with this file on particle board (usually do when I have some changes, instead of making oak sawdust), I did change the order to Vector selection and shortest path, We will try that to see if it makes a difference.. Thanks
 

·
Registered
Joined
·
349 Posts
One more problem that comes up now and then is the movement within the wood. When the wood is cut it will release tension that is built up with in the wood and the wood actually moves. Humidity can also cause newly cut wood to distort as it draws in moisture or releases moisture.
This was a flash back. I got a really great deal on some Red Oak and White Oak about a year ago. Let them acclimated in my shop with stickers. Month later I jointed and planed the wood, then cut blanks to size. Cut some cribbage boards and shortly after them coming off the CNC they curled enough that they never laid flat again. Found out after the fact that the wood was air dried and probably poorly. With kiln dried I never had the problem.

Steve.
 

·
Registered
Joined
·
21 Posts
Discussion Starter #13
I considered all the suggestions received here to try to remedy the problem... Two that I decided to act on were a loose coupler on the Z axis and reducing the plunge rate. I think it may have been both that were causing the problem, probably more so the loose coupler. I went over all the bolts I could get to on the gantry and the coupler on Z axis was the only place that seemed loose. Cutting the plunge rate from 30 in/min to 15 in/min seemed to make the cut run a lot smoother albeit it took a bit longer.
I also discovered I could raise the partition in the Linux cnc view to expose the text of the lines of code as they passed by, then I could easily spot the Z depth thru the cut and it was remaining constant as it should.
Seems I learn more about the whole operation when I have a problem :grin:

Thanks for helping me get thru this one!
 

·
Registered
Joined
·
16 Posts
I run a large Onsrud CNC for the shop I work in. I once had a problem with the "Z" cuts varying. Mine was actually a mechanical one not related to the collet the bit or the program. It actually was the mounting block on the top of the lead on the "Z" axis. It is bolted to the machine with two bolts. One of them was loose. When it plunge and then retract, the mounting plate was rotating just a little. Depending on how far it traveled, sometimes it moved a little and sometimes a lot. Tightening one allen head bolt fixed me right up.
 

·
Registered
Joined
·
1 Posts
Same Problem

I have exactly the same problem on my Laguna IQ CNC. I created 6 small signs to label my guitars. Each sign has some simple text and each sign is cut into the exact same size of MDF boards. The first 5 came out flawlessly. The 6th sign starts cutting and slowly goes deeper and deeper into the wood until about the fifth or sixth character it is so deep I have to cancel the program. After canceling I check my origin and X and Y are fine, but Z is now a good 1/4 deeper into the wood then it was when I started.

I wonder if a sensor is flawed. I am convinced that the problem is not in Vcarve Pro where I modeled the sign. And the material and backer board are clean and level. Simply stated, Z is wandering on me in the middle of a job!
 

·
Registered
Joined
·
3,727 Posts
Welcome to the Router Forums Marko1974. Please take the time to fill out your profile, it helps to know what kind of tools you have when we are trying to figure out solutions to problems.

It might help if we knew what CNC machine you have. If it is a small bench top unit you might be hitting the upper limit of your Z axis and losing the Z reading, then the CNC thinks it is higher and carves deeper. Could also be that the collet is not holding the bit correctly and be working its way down in the collet and carving deeper. Are you using the correct collet or are you using a reducer that is not holding the bit tight?

Pictures might also help us determine what the problem is.
 

·
Super Moderator
David
Joined
·
3,578 Posts
I have exactly the same problem on my Laguna IQ CNC. I created 6 small signs to label my guitars. Each sign has some simple text and each sign is cut into the exact same size of MDF boards. The first 5 came out flawlessly. The 6th sign starts cutting and slowly goes deeper and deeper into the wood until about the fifth or sixth character it is so deep I have to cancel the program. After canceling I check my origin and X and Y are fine, but Z is now a good 1/4 deeper into the wood then it was when I started.

I wonder if a sensor is flawed. I am convinced that the problem is not in Vcarve Pro where I modeled the sign. And the material and backer board are clean and level. Simply stated, Z is wandering on me in the middle of a job!
Welcome to the forum! Add your first name to your profile so it clears the N/a in the side panel. And like Mike said, completing the rest of your profile - location, tools, etc. - helps us to help you.

And photos always help! :grin:

David
 

·
Registered
Joined
·
65 Posts
I have exactly the same problem on my Laguna IQ CNC. I created 6 small signs to label my guitars. Each sign has some simple text and each sign is cut into the exact same size of MDF boards. The first 5 came out flawlessly. The 6th sign starts cutting and slowly goes deeper and deeper into the wood until about the fifth or sixth character it is so deep I have to cancel the program. After canceling I check my origin and X and Y are fine, but Z is now a good 1/4 deeper into the wood then it was when I started.

I wonder if a sensor is flawed. I am convinced that the problem is not in Vcarve Pro where I modeled the sign. And the material and backer board are clean and level. Simply stated, Z is wandering on me in the middle of a job!

Look at the coupling between the stepper and Z screw. If/when the fixing screws loosen, you get the symptoms you describe. When the spindle is commanded up, the screw slips in the coupling, so the spindle doesn't go as high as it is supposed to. However, when it goes down it is mostly coasting, so no slippage. Back up, slips again. Net effect is cutting ever deeper. Sometime you get a big slip, yielding a more dramatic plunge/depth of cut. Same thing happened to me once. Another possible source is you Z stepper losing steps. Usually, lost steps are indicative of binding somewhere in the Z axis.

Binding gives the same symptoms as a slipping coupling, and lost steps are also most common on the up move, since you are moving against all the weight of the z axis. For binding, be sure your linear rail bearing blocks are greased (assuming your machine has them). There are folks who don't know that they have to be kept greased. Without grease, they will self destruct. Ditto for Ball screws.

[If you find loose screws, especially on couplings, be sure to use blue locktite before you tighten them down. Otherwise, there is a high probability they will loosen up again CNCs have vibration, and that loosens screws. Blue Locktite is cheap insurance.

Gary
 
1 - 18 of 18 Posts
Top