PDA

View Full Version : lithopane sled making



luckettg
02-14-2014, 06:20 PM
I am having more difficulty making a sled for the acrylic than was expected. Using the Tips & Tricks (Lithopane (Lithophane) Carving 101) method of carving out a recessed region for the acrylic to sit it has presented some challenges. I am using the latest version of Designer. To my way of thinking, a straight router bit would be the best but Designer will not allow me to choose the bit and wants to do the cut with a carving bit, which is a hour or more. Best was over 3 hours.
In Designer, I first made a rectangle of the blank size, then a carve region, setting the depth. What am I doing wrong?

I can route a recess with my router in about a half hour, including setting up edge guides.

DocWheeler
02-14-2014, 06:27 PM
You are correct in thinking the straight bit would be best.
Use connected lines to draw the path you want the bit to take and then assign the bit.
Don't try to hog-out the full bit width, leave a little overlap.

fwharris
02-14-2014, 06:28 PM
If you are using a carve region that is the same as trying to carve a pattern and it will ask for the 1/16" carving bit. If you have the 3/16" carving bit you can change the default bit in the "board settings" "pattern bit" and it will speed up the carving time.

Another option is to set up a pocket cut using vector lines and select a straight bit. this would be the same as using your router to make the recess..

brdad
02-14-2014, 07:39 PM
This is one of the sleds I made for lithophanes using 3/8" flat bit for the recess and the 1/8" straight bit for access holes in the corners. Ya, the little corners do need to be cleaned off with a chisel - I could have fixed that, but it's easier to chisel.

luckettg
02-14-2014, 07:39 PM
I remember seeing that method before but not where I saw it. I have had my CW since 2007 but never have used this. Tips & Tricks or here in the forum? I am looking for the lesson now. Thanks for reminding me of the method.:D

SteveNelson46
02-15-2014, 08:24 AM
I am having more difficulty making a sled for the acrylic than was expected. Using the Tips & Tricks (Lithopane (Lithophane) Carving 101) method of carving out a recessed region for the acrylic to sit it has presented some challenges. I am using the latest version of Designer. To my way of thinking, a straight router bit would be the best but Designer will not allow me to choose the bit and wants to do the cut with a carving bit, which is a hour or more. Best was over 3 hours.
In Designer, I first made a rectangle of the blank size, then a carve region, setting the depth. What am I doing wrong?

I can route a recess with my router in about a half hour, including setting up edge guides.

A carve region will take a long time and leave the sides with a taper. A pocket cut is probably the best. If you have the 2D tools add-on you can use "Path Offset". Draw a rectangle the size of your blank. With it selected, select "Path Offset" from the tools menu. Offset the path to the inside the width of the straight cutting bit you plan to use minus a little for overlap. For example if you use the 1/8" cutting bit offset .1". Repeat this process until you get to the center. Assign the 1/8" cutting bit to all of the rectangle offsets and set the depth. Be sure to "inset" the first rectangle to compensate for the radius of the bit. For the 1/8" bit use .063. If you don't have the 2D tools you can use the grid to draw successively smaller concentric rectangles and then assign a bit. If you give me the size of your blank I will give you an example.

Smoken D
02-15-2014, 09:02 AM
When I made mine I just recall using a 10" wide x 18" long (7" rule) 3/4" MDF for a piece of 8x10 litho. In designer made a 8x10 rectangle, centered it on the 10x18 board and set a depth of .25 for the .25" litho. The litho fits in just right and use a screw driver to take it out after the carve. Believe the 1/16 carving bit what used and did not take very long to carve out. But I made it several years ago, still use it today. :)

SteveNelson46
02-15-2014, 09:48 AM
A carve region will take a long time and leave the sides with a taper. A pocket cut is probably the best. If you have the 2D tools add-on you can use "Path Offset". Draw a rectangle the size of your blank. With it selected, select "Path Offset" from the tools menu. Offset the path to the inside the width of the straight cutting bit you plan to use minus a little for overlap. For example if you use the 1/8" cutting bit offset .1". Repeat this process until you get to the center. Assign the 1/8" cutting bit to all of the rectangle offsets and set the depth. Be sure to "inset" the first rectangle to compensate for the radius of the bit. For the 1/8" bit use .063. If you don't have the 2D tools you can use the grid to draw successively smaller concentric rectangles and then assign a bit. If you give me the size of your blank I will give you an example.

Here is a link to a short video (no sound) using the grid method.

https://drive.google.com/file/d/0B0jR3LNRxqJeYXlQOXRsXzBnUXM/edit?usp=sharing

henry1
02-15-2014, 10:01 AM
Here is a link to a short video (no sound) using the grid method.

https://drive.google.com/file/d/0B0jR3LNRxqJeYXlQOXRsXzBnUXM/edit?usp=sharing
Thank you steve I have been wanting to know this one I did forget about this I never think of using the grid

luckettg
02-15-2014, 04:46 PM
I decided to just let the machine use the 1/8 ball end bit to make this cutout. Everything was going well until it tried to get the bit position. The little flapper came out and the Z axis looked like it was over driving down, pushing the flapper down, then stalling. The LED says "Z Axis Stall, Err E06-0324. Press STOP". I am beginning to regret upgrading to the 2.004 version as the machine was at least working well with the 1.181(? latest old version what ever that number is). I am not sure how to proceed with this now.

fwharris
02-15-2014, 05:25 PM
Post your mpc so we can look at it. Are you using CarveWrights 1/8" bit?

luckettg
02-15-2014, 05:46 PM
Yes, the short 1/8 bit that came with the CW set. I have not used it prior to this. I ran the X, Y, Z, and cut motor tests. They all homed and functioned correctly.

fwharris
02-15-2014, 05:58 PM
I did not see anything unusual with the mpc. Looks like you are using 3/8" material according to the carve region depth.

What quality setting did you select when up up loaded to the card?

Did you try running the project again?

luckettg
02-15-2014, 06:26 PM
Yes, to your questions, and I may have figured out what is happening. The earlier question about the bit made me start thinking if my memory was right. It was not. The bit is longer than the 1/16 ball nose or the 3/16 ball nose. It came from Soigeneris, where I have been getting bits for a while. This 1/8 ball nose, #CM404-1250-100B, is a new type for me to try and I had forgotten about it. I am selecting the long 1/8 bit now and will give it another go and will report back. Every time I stop using my CW I have another learning curve to climb when getting back to it.

luckettg
02-15-2014, 06:31 PM
Ok, choosing the long 1/8th bit solved the homing problem. It homed correctly, then wanted me to load another 1/8th deep carving bit. I do not know enough about this newest deep carving feature, stopped it there, and am getting ready to go back to a 1/16 ball bit. Not much difference in carving time, both just under 2 hours. It will be a good test of the machine I guess.:)

fwharris
02-15-2014, 06:35 PM
Yes with the new 2.xx version it is expecting the bit to be certain length +/- and will give the stall error if it is not.

luckettg
02-15-2014, 06:46 PM
I am wrong again. My original 1/16 bit is the same length and fluting as the 1/8 ball nose. I have been using shorter 1/16 bits but that is in the shank, not the cutting area. With the bits I have been using, the CW overdrives the Z axis. It is definitely a problem with the software I think. The 3/16 ball nose that came from CW is a short one similar in length to the replacements I have been getting in the 1/16 ball nose carving bits. I am using a Rock Chuck with the 1/2 adapter, and have been using that for several years without any problems. This homing problem has shown up with the Designer 2.004 upgrade I did a couple of days ago.

fwharris
02-15-2014, 07:30 PM
A lot of people with the rock have fallen back to 1.xxx until the software lords can get the bit find problem corrected..

luckettg
02-15-2014, 07:41 PM
Can I do that too? I shall give that a try. Thanks!

fwharris
02-15-2014, 07:54 PM
Can I do that too? I shall give that a try. Thanks!

You should still be able to, when you installed 2.xxx it was not installed over 1.xx so if you did not remove it you should still have the program.

luckettg
02-15-2014, 08:37 PM
Yep, once I went back to the old Designer, the problem went away. Too bad, as I really liked the new features on version 2. I hope CW will fix the issue and not force us all to get rid of the Rock Chucks. If CW had addressed the problems with that piece of crap original chuck, and in a timely manner, I would never have bought someone elses. The way they handle this issue will be a deciding factor in whether I buy a second CW or a flat bed CNC. It certainly is keeping me from buying any more software add ons at this point too.

luckettg
02-15-2014, 10:00 PM
The sled just finished but is not exactly to the dimensions I wanted. Instead of 12x6 it is 12.125x6.125. The depth is close to the 3/8. Turns out my acrylic is slightly under 3/8 so must actually be a metric dimension. I will be inquiring to the supplier about this. Their 6x12 is slightly under that. I will use shimming to place the acrylic blank into the sled and give it a go tomorrow. It is nearly 11pm and I am tired. Thanks to each of you for your help. This forum has once again proved its worth to me. I hope CW gets the software fixed soon as I do not want to have to learn how to use a flat bed cnc unless I really need to. Good night all.:)

aokweld101
02-15-2014, 10:35 PM
I am curios as to witch of the patterns works best and is the easiest for the pockets cuts I didn't finish the pattern but it to give you an idea...It seems to me that if you do the rectangle as a individual cut on each rectangle the bit would lift up and back down..

fwharris
02-15-2014, 10:48 PM
The difference could be the taper on the bit I am guessing. When you go to carve you will probably want to jog the bit over so it touches on the acrylic and not on the board since is less that 3/8". When it does the "finding surface" step press the stop button once and select #1 jog. Use the arrow keys to move the truck into position over the acrylic..

aokweld101
02-15-2014, 10:50 PM
I assigned the .125 cutting bit for the pocket cuts . What I'm asking is a cut path better..... or making the rectangle as cuts does the bit stay down... or lift up and down for each rectangle, I also made the pocket cut .25 deep.

SteveNelson46
02-15-2014, 11:36 PM
The difference could be the taper on the bit I am guessing. When you go to carve you will probably want to jog the bit over so it touches on the acrylic and not on the board since is less that 3/8". When it does the "finding surface" step press the stop button once and select #1 jog. Use the arrow keys to move the truck into position over the acrylic..

I think the question is which is better, a series of concentric rectangles or one continuous spiraling line. I think one continuous line would be better as long as the bit doesn't take to much bite on each pass. No lifting of the bit. It's a little more difficult to establish an exact outside perimeter though.

bergerud
02-16-2014, 12:03 AM
I am curios as to witch of the patterns works best and is the easiest for the pockets cuts I didn't finish the pattern but it to give you an idea...It seems to me that if you do the rectangle as a individual cut on each rectangle the bit would lift up and back down..

What I do is start from the inside and spiral out and finish by going around the boundary. The bit stays down on one path the whole time. I try and cover as much as I can with y paths. I use a fine 1/16" or 1/32" snap grid to draw the cut paths.

Here is an example of some pockets from my rotary jig project. (Toggle non end points to see where they start and stop.)

fwharris
02-16-2014, 12:14 AM
I think the question is which is better, a series of concentric rectangles or one continuous spiraling line. I think one continuous line would be better as long as the bit doesn't take to much bite on each pass. No lifting of the bit. It's a little more difficult to establish an exact outside perimeter though.

I do agree on that point. They are not as easy to lay out and probably why I just use the offset tool. A trade off between design time and a small amount of carve time I guess..

aokweld101
02-16-2014, 09:11 AM
Thank you, it was the first time seeing it done with the rectangles I have been doing cut paths working from the center out with the offset and like you guys said it is the last cut around the pocket cut that I have to adjust my grid to make it work. thanks again!

luckettg
02-16-2014, 10:30 AM
I might try this on the next sled cutout, adjusting the sizes to fit mine.
What are the little risers for?
Did you set up the rectangles as cut paths?
I have gone back to Designer 1.187 since the 2.004 version will not home the Z axis correctly.


This is one of the sleds I made for lithophanes using 3/8" flat bit for the recess and the 1/8" straight bit for access holes in the corners. Ya, the little corners do need to be cleaned off with a chisel - I could have fixed that, but it's easier to chisel.

luckettg
02-16-2014, 10:34 AM
I am on a mission to get a couple of lithopane projects done before next Thursday, but this cut path stuff is drawing me away. It is really interesting and I want to play with it. Thanks to all for bringing it up. I have been making signs for several years and not using the cut path since about 2008. Now I am inspired again! :D

bergerud
02-16-2014, 10:47 AM
Why go to the trouble of milling out a pocket? Surely the plastic does not need back support. Why not just do a cut out with a ledge?

fwharris
02-16-2014, 11:06 AM
Why go to the trouble of milling out a pocket? Surely the plastic does not need back support. Why not just do a cut out with a ledge?

Dead on Dan, that is how I did mine..

luckettg
02-16-2014, 11:49 AM
Interesting idea and simple to make with a saw and a router...much quicker too. It took nearly two hours to carve the 6x12 pocket. I wonder how long it would take for the CW to do the cutout and ledge?

bergerud
02-16-2014, 11:58 AM
The CW will cut out the ledge and the hole in only a few minutes.

aokweld101
02-16-2014, 02:17 PM
I have been interested in the pocket cuts and the cut path I have been sitting here for the last 3 hrs. laying it out I have done the pocket cuts on a project for a mirror on the paddle head that elamb posted on the forum and think I lucked out on it. On the litho insert that I had just done the outside edges were a little difficult to maneuver but I figured it out on manipulating the grid to get it to the size. Used .125 cutting bit and .25 deep If any one see's something wrong please tell me...I am going to lay it out using the .375 cutting bit and make it do two passes for the depth at .125

bergerud
02-16-2014, 03:34 PM
If the pocket is just for a mirror, make the paths 1/8" apart. It may require a little clean up but so what. Also, I think I would just have gone back and forth cutting in the y direction and then around the perimeter. (Like the larger pocket I posted.) Always think about minimizing the x movement.

aokweld101
02-16-2014, 03:48 PM
thanks Dan, it would be a lot easier doing the parameter last and doing strait lines in the y direction I've learned two things on this post...see I always try to out think myself sometimes, that took a long time laying that out it's always the easy solution that's the hardest....

luckettg
03-02-2014, 08:23 PM
I set up a series of rectangular cut paths for my next sled but am dismayed that it still wants over an hour to do it while using a 3/8 straight bit. I suspect I am doing something wrong. I also set the maximum cut to .125 per pass, and a .25 depth, then dropped the maximum limit. It changed the carve time from 1:24 to 1:02, not a big improvement. Removing the corner circles only saved a couple of minutes. What do you all think??:confused:67934

bergerud
03-02-2014, 08:49 PM
I think rectangles are poor. The bit plunges in and out for each one. Also, most of you cutting is in the x direction. Better, I think to snake back and forth across the board. Remember also that the direction you draw the path will be the direction the bit follows. I like to snake back and forth to clean out the interior and then go around the perimeter. All one path.

luckettg
04-20-2014, 11:31 AM
I discovered that the plastic does need back support, else it bends down when the bit is pressing and causes lighter cutting than it should have. The effect is like it is floating. I am looking into some sort of vacuum clamping. Anyone tried that with the CW?