Phill Anton Consulting's OG and S081 Franklin door profiles in Mozaik are marked "Frost Labs only" because their corners need an 8th-inch ball-nose mill to clean them out. The full process is: import PAC's panel tool group and door files into Mozaik, build the order with the S081 Franklin tool group, generate G-code, then upload that G-code (plus your tool library and machine settings) into Frost Labs and run its auto 3D corner shaping. This note walks the setup start to finish.
Why do some PAC profiles require Frost Labs?
Any door profile on phillanton.com that says "Frost Labs only" can't be finished on the router alone. The profile corners need an 8th-inch ball-nose mill to come in and clean them out, and that ball-nose pass is driven by Frost Labs' auto 3D corner shaping rather than by Mozaik directly. The OG profile and the S081 Franklin profile (the one demonstrated here) both fall into this category. A 30° V-bit is optional but Phill recommends it because it gives cleaner corners and makes the finishing process easier.
How do you import PAC's tool group into Mozaik?
First unzip the download: open your Downloads folder, find the PAC zip file, right-click and "Extract All," and extract it there so you have the unzipped folder. In Mozaik, open the optimizer, then go to Libraries > CNC tooling > Panel tool groups and choose Import. Decide which mid-size down-shear you run first — 3/8", 7/16", or 1/2" — and import the matching panel tool group from the download (the demo uses the 1/2" down version). When Mozaik asks to update because the placeholder tools already exist, say Yes.
How do you swap the placeholder tools for your own?
For each placeholder tool, left-click it twice to replace it with a tool already in your tool set:
- 1/2" down-shear — replace with your existing 1/2" down-shear.
- 5/8" panel bit — if you don't already have it, go to Tool properties, find the 5/8" panel bit, and rename the tool to remove the placeholder portion of the name.
- 8th-inch down-shear — you probably already have this.
- 30° V-bit — optional for this profile, but recommended for cleaner corners; left-click and select your 30° V-bit.
Important note from Phill: as long as your tool heights are correct on your machine, what you see is what you get — the on-screen profile will match the cut result.
How do you import the PAC door files?
Back in Mozaik, go to Libraries > Doors, into a standard (library) and into Routed, then import the door files. From the same unzipped download, open the door files and pull in all six profiles (the demo pulls in just the Franklin door for the example). The margins come in already set — accept them and say OK.
How do you build the order for the S081 Franklin profile?
Go to the Order tab — note this switches the room you're in (Order Entry). Select the proper library (the standard one), then choose the Franklin door. Set the door to use the pocket tool, at which point the selected tool group is S081 Franklin; say OK. On the Order tab, confirm the profile matches the door style, set a typical sample size of 12 x 15, go to Cut List, then back to Order Entry and choose Optimize. Then reopen the optimizer to finish.
What two tools do you create in CNC tooling before G-code?
In the optimizer go to Libraries > CNC tooling. Two things remain:
- Make the 8th-inch ball-nose mill. Copy your 8th-inch down-shear and name the copy "8th ball nose." Make sure Dado is not selected. Go to CNC door tool shape, click the bottom-right point, and set the radius to 0.0625 (i.e. 1/16") — type it, hit Tab, say OK. That radius is what Frost Labs reads to detect the tool as a shaping tool.
- Put the called-on tools into your tool set. Tool sets vary by shop, so swap as needed, but you must have in the set: the ball-nose, the 5/8" panel bit, the 8th-inch down-shear, and the 1/2" down-shear. The ball-nose in particular has to be in your tool set.
Optimize the material, then run a simulation to check it.
How do you fix the "no pocket found" / pocketing tool error?
If the simulation fails with "no pocket found on this tool on this door," your pocketing tool isn't set as a pocket — common on older Mozaik versions where the pocketing tool isn't selected as "pocket." Go to Libraries > CNC, back into your tool set, and bring in a pocketing tool. In the demo Phill adds a dedicated pocket bit, which is already selected to pocket. When generating G-code, also confirm your 30° V-bit is in the set (Phill had to add his back in). The final calculation for G-code uses the pocket bit, the 1/2" down-shear, the 5/8", the 30° V-bit, and the 3/8" compression bit for cutout — the ball-nose is not in this list because at this stage you're only making G-code, not the shaping pass.
Where does Mozaik save the G-code?
Create the G-code, then locate it under Mozaik's shared files G-code folder (job G-code). You'll upload this file into Frost Labs next.
How do you set up Frost Labs and run 3D corner shaping?
- Open Frost Labs (after starting your free trial) and Refresh. Go to Cabinets.
- Upload your tool library: go to New > Tools and tool sets and upload your tool library. Find it in your Dropbox under the Mozaik shared folder > data. If you don't use Dropbox, it's on your C: drive under CNC > Tool Lib.
- Upload machine settings: go to New > Machine settings, back to the data folder, and select your machines settings file.
- Select Auto 3D corner shaping, then choose the machine you're using and the correct tool set. Your ball-nose appears under "for shaping" because it has a radius, so Frost Labs detects it.
- Switch from Simple to Advanced view (View > Advanced) if you don't see the advanced settings. The only thing to change is the tool height adjustment: set it to about 0.02 for this profile. That adds a little extra to sand off in case the Mozaik tool geometry isn't perfect; at 0.02 you can typically double up a 120-grit disc and sand it by thumb for a few seconds. Setting it to zero makes the ball-nose cut exactly on the line.
- Make sure Raised panel and Glass cutout are selected.
- Upload your G-code file (job G-code folder). You can upload individual files for a single job or a zip file. Click Execute — it loads everything with a progress percentage, then asks where to save the output.
From there the run is machine-specific.
How do you sanity-check the G-code before cutting?
Always check the G-code so nothing plunges through your spoil board (Phill hasn't seen issues but treats this as a safe-bet habit). Open the G-code (the demo's is for a Shop Saber) in a G-code decode viewer and look at the Z values for the ball-nose. The ball-nose is in slot 12, so search for T12 to find where it's picked up. In the example it never goes below approximately 0.51" above the spoil board, then works its way up around the four corners; after the corners, T2 is the cutout bit. If the corner shaping looks wrong, the culprit is usually the tool height adjustment — sneak it a little closer. If that doesn't fix it, close the optimizer and re-upload your most recent tool and machine settings files, since Frost Labs reads the saved versions.
Get it done-for-you
You can set this up by hand (above). If you build these regularly, the PAC Mozaik Closet Library from PAC has it ready in Mozaik. → phillanton.com
Full disclosure: Phill Anton Consulting makes this product.
FAQ
Which PAC door profiles need Frost Labs in Mozaik?
Any PAC profile on phillanton.com marked "Frost Labs only" — it needs an 8th-inch ball-nose mill to clean out the profile corners. The OG and S081 Franklin profiles are the examples shown here.
What makes Frost Labs detect a tool as a shaping tool?
A radius. You copy your 8th-inch down-shear into an "8th ball nose," set its bottom-right point radius to 0.0625 (1/16") under CNC door tool shape, and Frost Labs reads that radius and lists it under "for shaping."
Why isn't the ball-nose in the G-code tool list?
Because the Mozaik G-code stage only handles routing/cutout (pocket bit, down-shears, 30° V-bit, 3/8" cutout). The ball-nose corner shaping happens later in Frost Labs, driven by the same G-code.
What does the Frost Labs tool height adjustment do?
It leaves a little extra material to sand off in case the Mozaik tool geometry isn't perfect. About 0.02 is good for this profile; zero makes the ball-nose cut exactly on the line.