what are these lines

[POPS 64]

Can someone tell me about these vertical lines in my carving? This is the second carving I've had this on. I don't know if it"s me , the machine or a corrupt file . these files came with the machine from SB. I'am leaning towards corrupt .21024

21025

21026

21027

[supertigre]

I had a similar issue a few years ago and the issue was the control software. What version of ShopBot control software are you running?

[srwtlc]

What type/size tool did you use for the roughing pass and then the finish pass? What were your toolpath settings also. Looks like the roughing pass, with a flat end mill, may not have had enough machining allowance. Did the preview look the same? It has very poor detail also, as if it was done with too large of a ballnose for the finish pass and maybe too large of a stepover %.

[POPS 64]

It was done with a 1/8 ball for rough , 1/16th taper for finish i dont think its setting because everything else i carve looks great I did this one twice and it did it both times and I carved ir different sizes and both matched and the preview looks fine. There was another in the library that this happened to. partworks and
pw3-d

[Brady Watson]

You should be rastering with the grain, not across it. Going across the grain can result in tear out especially in maple. Also, running too aggressively with not enough RPM will cause that kind of finish - particularly if there is a fine detail texture in the background or little details you need to pick up. You really don't want the Z hammering up and down or you'll carvings that look that way.

You should be cutting that relief on the finish pass no more than 3,2 or 2,1 if the details are very fine.

What speeds & RPM were used on the finishing pass? How much allowance (meat) was left between the roughing & finishing passes?

-B

[POPS 64]

Brady my router alwayys is at 24,000 I've never tried to change my speed on anything I've done 30 3-D carvings and even more lithophanes and have had this only twice. on wood I always use factory settings , Ive made some changes on the litho's but had help. I inherited my machine and new nothing about this stuff when I started . And havent had any quality issues really except for this and one other file. the other file left holes all other it like a drill bit went across . what did you mean 3-2 , 2-1 I'd like to learn more . Especially if i can make things look more crisper. thanks

[POPS 64]

Brady I just looked at the file and a few others and all the speeds call for 12,000 rpm mine is always at 24,000rpm I was told to always leave it on high. what is the best thing to do follow the file ? And is it best to rough across the grain and finish with the grain ? And on the finish pass will changing the stepover give a better detail? I change it up on the lithophanes .

[Brady Watson]

Jeff,
What move speeds were used to cut the finishing pass? E.G. - MS,3,2

-B

[POPS 64]

Brady , i dont know what those letters and numbers are your asking for or to to find them. finishing pass - E. G. MS 3. 2. ????

Here i went through the steps to run it. in the funish i brought up edit bit
.0625 taper ball nose , pass depth .05, stepover .005 8% , feed rate 2.
plunge rate. Sorry I 'am not more help . I learned how to run this out of a notebook that told me how to load files and turn it on and run . I 'am learning as i go almost everything turns out great. havent had anyone to teach me so the technical part I dont know.Especially talking it. thanks again Jeff

[Brady Watson]

Jeff,
MS = Move Speed in SBP language. You can find it by looking at the speeds you have set in your SBP toolpath that you created for the finishing pass.

E.xample G.iven : MS,2,1 = Move Speed for XY = 2 & Plunge Speed for Z = 1 Inch Per Second.

It appears to me that the finishing tool was not fully contacting the top surface of the relief - only partially machining it. I say this because it appears that there are gouges on the surface consistent with 1/8" ball tool marks. This can be caused by using the Zzero plate for the 1/16" finishing tool in a different location than the 1/8" roughing tool.

Also, if you used an 1/8" ball with a 3D finishing toolpath with zero allowance (Aspire usually leaves .04" of meat on a roughing pass for the finishing tool to shave off) - and your Zzero location was different from one tool to another, then it is possible for the finishing tool to start off a little higher in Z than it should. Furthermore, material moves & depending on how you were holding this down, it is possible for it to move, twist or warp after all of that material is eroded away.

Have a good look at the part again & see if this is a possibility.

-B

[Joe Porter]

Jeff, if this files came with the machine, they were already toolpathed using certain shapes and sizes of bits. Only the feeds and speeds can be changed. Why don't you go back over the original file and see what tool was chosen and use that one. If this was done by Vectric, as usual, they hardly ever use a 1/16" tapered ball nose. Usually on a dished model like this, they use a 1/8" ball nose and do a finish toolpath only and the dish is always even with the top of the material. The feeds and speeds can be changed to suit you and the machine. Maybe 24,000 rpm is a little high, mybe 12,000 would be better. Hope this helps...joe

[POPS 64]

Brady I see what your saying but, you need to know I run that machine 4-5 days a week carving signs making boxs , doing lithophanes , applicays , rosette's , and whatever else I can think of to try . all my files came from shopbot when machine was bought. All the files V3m when I go to use them call for a 1/8" ball nose for roughing , then a 1/16" taper ball nose for finish and like I said this file and the one with children's building blocks is the other that mess's up . Everything else is great I've never had a complaint about any of my carvings. Now maybe when my brother bought the machine he programed the 1/16 into the system. I dont know but everything I do has a rough and finish except when doing script.Sorry not trying to be diffacult but its only the 2 files that dont work . And I only use the bits PW-3D , Photo V carve call for, I only pick bits on things I desgn. thanks again

[cowboy1296]

I always use a 1/4 inch ball nose for roughing with a 40% step over no matter what size the file is. a feed rate of 3.3 inch per second and a plunge rate of about 2. I cut fairly shallow with depth of cut set at .075 in my tool path data base. It seems that a 1/8 inch roughing would double your machine cutting time but you could be cutting deeper than me.

Now one way to choose which ball nose to use for the finishing. Calculate it first using a 1/8 inch ball nose and preview the tool paths. Leave that preview on your screen and then re-calculate it with a 1/16. Watch your screen closely and then click preview. Depending on the speed of your computer you should notice a quick change in the preview. If it is a major change meaning better quality then use the 1/16 inch bit, if not much of a change use the 1/8.

[POPS 64]

Rick I'll try itt but I've never done a finish pass with anything but a 1/16 tapered ball nose . Even on lithophanes . I only use ball nose for roughing.

[cowboy1296]

It all depends on the size or detail of your file. I do some large plaques using a 1/16 but then others a 1/8. the preview is the tell all on which to use.

[Brady Watson]

Just re-toolpath it. Seriously. I thought something was wrong with your machine & it was important. :rolleyes:

Reload the 'Getting Carving Quickly' CD if you are concerned about it being corrupt & then create fresh toolpaths. 'Mystery' solved.

-B