Ok, I have a confession to make. The only way I’ve been able to consistently cut profile cuts is to trick the Multicam. I bring my own 1/4" or 1/2" sheet of MDF and use it as a sacrificial spoilboard on top of the Multicam’s spoilboard and put the material to be cut on top of that. Then I set the surface block on a piece of scrap that is thinner than my sacrificial spoilboard and set my max depth to the top of the scrap. I’ve tried both the methods of setting surface and max depth–the kind Chris teaches in class and the Klasmer (sp?) method–and neither works unless I set max depth below the bottom of my material. If I don’t resort to such trickery, my “through” cuts leave nearly 1/16" of material. Obviously, this seems nuts to me. Can someone tell me what I’m missing?
Have you set your maxdepth to just past the Z via a relative value? The spindle won’t go further than the zero from the puck, and will cap out before it tries to go for what you really set versus going through your material.
It’s the only way I’ve gotten reliable profiles
I have, but Vcarve bitches like a mofo when you do it. Should I just ignore the warnings in Vcarve?
I was told by someone outside the Makerspace (and you know him ) that the Klasmer method was the way to go because it eliminated the question of whether I properly measured the thickness of my work. But even using that method didn’t result in complete through cuts. It just seems that something is out of adjustment. That’s why I’m putting this out there.
Definitely make sure your G-Code goes deeper than the thickness of your material by a little bit. I typically do this by telling V-Carve my material is slightly thicker than what I have measured if a profile is involved.
Then when you set your max depth and run your program, you should definitely see the UI on the pendant at some point say in green at the bottom of the UI something like “max depth active”. This lets you know it’s going as far as it is allowed to go down. You don’t want to go crazy with the G-Code going too deep because then you’ll do things like extra passes you might not need or blow out tabs you might have wanted etc.
Interesting. My method created a false max depth on the Multicam. Your method uses a false thickness in Vcarve. I’ll give your method a try. It seems safer to have the Multicam know exactly where the real max depth needs to be.
How much do you add to the thickness of the material in Vcarve? My through cuts (before trickery) have been off as much as 1/32" or even 1/16", which seems like a lot to me.
I feel like I used to just add 0.1" (just lazy typing). The biggest danger is if that number is bigger than the thickness of tabs you might want, those tabs won’t be there at all
Obviously try to measure what you have too with some calipers. The ambiguity in advertised size usually works the other way though. 3/4" plywood for instance is usually actually 18mm, which is something like ~0.709" instead of 0.75". Of course you might be dealing with more reputable Balts who make it 19mm?
Also, be sure you are setting max depth with the hold down vacuum on. Otherwise, when you turn it on, the LDF may compress some, leaving uncut material.
It’s Fasmer. And Fasmer does not set Max Depth … it sets Z=0 at a calculated top of surface level you specify. If you independently set Max Depth and use Fasmer to set top of surface, you will need to get your math right. At DMS I always encouraged users to cut to, not past the spoilboard simply because maintaining the spoilboard is a huge pain. On my personal CNC, I routinely use the Fasmer method to set the top of surface Z=0 value and then cut 0.015" deeper than the material thickness specified. Example: cutting 18mm ply, set top of material to be 0.71" above the spoilboard, and specify Aspire/VCarve to cut 0.725" on thru cuts. I do this because I know the guy who will have to maintain/resurface/replace the spoilboard (me) and fixing my own stuff works for me. It’s just doesn’t work as well in a shared environment like DMS where a cut spoilboard is the next user’s problem.
Good point from @kbraby that the hold down vacuum should be on when setting Z. It can be more than LDF compression … the spoilboard can be warped upward as well.
Check to see if this is consistent at different points on the table. In the past, there were areas of the table that simply would not stay flat (front right corner was notorious for this) and if you set Z there, it would not yield consistent results.
Do you know if the entire spoilboard has been surfaced? If someone surfaced only part of the table, you will have inconsistent spoilboard zone heights.
Hope something in the above helps.
Added thought: Make sure someone hasn’t “recalibrated” the touch pad height. If the pad actual thickness doesn’t match what the machine has been told it is … that’s a problem. @themitch22 can help verify the correct value is being used.
The surface block is calibrated correctly, I checked.
This is is partiallymy fault. The Z axis physically reaches its limit before shorter bits can reach the spoilboard.
Right before the covid lock down, I replaced the spindle and when I installed the new spindle I mounted it to the spindle plate on the upper set of holes which lifted the spindle about an inch or two higher than normal. Because its a major pain to tram the spindle, I haven’t had a chance to fix the issue.
In a way it does help prevent people deep diving into the spoilboard accidentally, but I’ve encounter issues trying to plunge small bits deep enough. It doesnt warn you if Z+ max limit is reached it just won’t go farther.
I plan on fixing the spindle soon, I just need to find the tramming dial indicator in machine shop again and spend a good 2 hours. I am helping someone on it Sunday so I’ll probably do it then.
In the mean time, using your own spoilboard to raise your part to profile cut is recommended.
You can “Adjust Max Depth” by pressing shift ^ and max depth button, then Z up and down to adjust the max depth value (positive is down, negative is up), this will allow you to have Vcarve actually plunge further into the material. And Bert is right the spoilboard marking is the next person’s problem (I’m guilty of this, but I plan to resurface the spoilboards)
Also you can adjust surface in the Utility menu but really that’s won’t help you except for fancy engraving work. Fasmer surface is definitely more advanced user I personally don’t use it for routing, especially with the warped uneven spoilboard
“Fasmer”, that’s it. I couldn’t remember the name. I don’t know where I got “Klasmer”–except perhaps from the style of Yiddish music (Klezmer).
I did have the vacuum on when I set the surface height. I’m usually cutting on a 2’x4’ sacrificial MDF spoil board that I align with the front right corner using one of the big right angles hanging on the wall. I set the max depth somewhere outside of my MDF spoilboard.
I’ll keep using my sacrificial spoilboard (I wonder why this isn’t taught in class?) and tweak my Vcarve model a bit before my next attempt.
@themitch22 - The bit I was using was a new 3" long 3/8" Amana compression bit, so “small bit” wasn’t the problem.
Your method is a good one for protecting the spoilboard. The Cons include: reduces the vacuum holding force on the work piece and elevates the work piece which can become a problem with long bits and tall material.
It’s all a balancing act where you try to find the sweet spot amongst the competing objectives.
Well, after some experimentation, I think I’ve finally solved the problem in a way that will work more consistently, and I thought I should report back.
I tried the method that @Kentamanos suggested and I saw “max depth active” during the profile cuts, but there was still an irritating amount of material left. In the attached photo, see the two frames on the right. The top photo shows the front and the lower shows the back, where you can just barely make out the light coming through the bottom of what should have been through cuts.
In the next attempt, I created a test circle tool path in an unused area and adjusted max depth until it just cut all the way through. In some areas it still left an onion skin of material, but that was no problem to clean up. In the lower left frame you can see the back of the material, and the top left frame was my final max depth adjustment.
Because of how our spoilboards are used, I suggest we start training users how to mill spoilboards. MDF is cheap and in circumstances where we need to use a spoilboard as a spoilboard (going deeper than the material for profile cuts) but not spoiling it for the next person.
I always set material surface and bottom with the pendant and tell VCarve to cut deeper than the thickness of the material. For example, on 18mm plywood I’ll tell it to cut 0.75" for a profile. This always results in the the “Max Depth Active” notice on the pendant and makes tabs somewhat thinner (by ~0.04").
If I need something really clean I’ll put a piece of MDF under my work and cut into it. That has the advantage of allowing me to use a single downcut bit for the entire job since the lower surface is 100% supported by throwaway MDF.
Yes, this is exactly what @Kentamanos suggested, but it didn’t work. (See two frames on right side of my picture.)
I have used this method successfully as well, but as @bertberaht pointed out, is that there is some vacuum loss (and it is a bit of a pain to drag along a sacrificial spoilboard along with everything else).
Adjusting the Max Depth yesterday seemed to work quite well, although it required making some test cuts first.
I’m surprised that you didn’t get any breakthrough at all. Usually at worst I’ll have part of a job with a thicker onion skin because the spoilboards aren’t completely uniform. Setting max depth with the vacuum off will also result in more material left uncut.
When using my own spoilboard I generally pin my work to it using a 23 gauge pin nailer in areas I know are waste.
When I brought my own sacrificial spoilboard, I found a slip of wood or some flat material that was a 1/16"-1/8" thinner than my spoilboard and set max depth on that. That was the only way I could get consistent through cuts before I figured out how to adjust Max Depth.
Perhaps something has changed. I’ve always had reasonable luck with the methods described earlier. In any case, issues like yours are one of the reasons I’m building a CNC router for myself (leave it in place jigs and fixtures being a primary one).