Production Level Vac Fixture

[Adam Bullington]

Hello All,

I am in progress of getting my production vac fixture designed and cut out. I plan to cut the prototype out of MDF and then switch to another " still undetermined " material for the final permanent fixture board. let me know your thoughts this board will hole (9) 11"x14" solid wood blanks to be machined 9 at a time. Let me know what you think good or bad. This is the only picture i have of this prototype at the moment due to my minimax sliding table saw attempting to catch fire on me while this was cutting so I was a little sidetracked during the initial cut. But this now has the center hole cut out and a gasket groove between the outer profile and the grid pattern and the grid has been machined down to .05 thickness to allow the outer edge to "capture the blanks" and assist with horizontal movement and the vacuum will cover the vertical movement. Let me know what you think. Thanks
IMG_2847.jpg

[Brad Shipton]

I gather you are using your F4 vacuum. How thick is your material that you are cutting? The basic concept will work fine, but it seems more complicated than it needs to be. If you look at the top of the page (http://www.allstaradhesives.com/) on the allstar site you can see some examples of dedicated fixtures for in-board gasket applications. If your stock is say 3/4" thick you will not need all that interior support grid system. Anywhere your stock touches the MDF reduces the surface area for hold down, and given your vacuum is limited to about 10" Hg, that might end up being important. I would paint this test jig, and try cutting some parts to make sure you have enough hold down.

You need to make sure to prep your stock as near to perfectly flat as you can. Any amount of curvature will cause problems achieving vacuum. This fact is why all star has so many different gasket thicknesses and densities. I had some stock that had been sitting on a rack for a while that had small amounts of curvature (1/16" or less if I recall correctly). It caused me a lot of headache as my vac could not pull it flat.

For substrates you can add paint, cover sheet, plastic, aluminum or Medex. I have had okay luck with Medex, but on my last project I could not get above 15" Hg. Not that it matters here, but Medex taps fine if you are careful. If you mess up your threads you can add a bit of epoxy.

[Adam Bullington]

Brad,

I am using the F4 Vacuum, The material I am machining is .75 white oak and all has been planed and sanded thru a wide belt to .75" these blanks consist of 3-6 edge glued strips with a industrial titebond glue. "I think the white stuff"

[Jim Becker]

One suggestion I have is that the border exactly match the size of the plaque blanks (I assume it already does, but...) and that you slightly lower the standoffs in the middle so that the edges of the plaques are slightly below the surface of the fixture. That will provide additional lateral support while cutting. Just be sure to account for that height difference in your toolpath design. Otherwise, that looks like a nice production setup.

[Adam Bullington]

Jim,

They are currently, Ill try to post another picture of the final prototype the overall pocket is .25 deep and the standoffs are at .20 deep or .05 off the bottom, with the gasket slot cut at .19 deep into the bottom of the .25 deep pocket to allow the .25 x .25 gasket to stick out .01 above the standoffs so with vacuum compression everything should settle up nice and flat with each other. " hopeful thinking" anyway..lol

[Brad Shipton]

It is easy to worry a bit too much about lateral movement. I like to oversize my blanks a bit extra and allow myself the flexibility of not being too accurate how they are cut. In your case with only 10" Hg it might be more important, but that will depend on how aggressive you are cutting. Here is an example of mine with zero lateral restraint. In this case I was cutting out face frame parts. Each pod is 3"x4", and I am using the 1/32" medium allstar gasket material. I only added the center two pods after seeing a bit too much vibration as the parts were being cut. I cut 40 frame parts this size, 25 shorter, and 12-8'-0" tall frame parts. I lost one part because I was trying a single flute bit and did not have my settings quite right.

VAC-JIG.jpg
FF-cut.jpg

COMPL.jpg

Do you have access on all four sides to your table? If not, you might want to think about how you load the parts. I have good access on two sides, so I tend to load off the end or one side only.

[Adam Bullington]

Brad,

I have access to 3 sides fully on my machine for small parts and two sides fully for sheet materials. As far as being aggressive this production setup is for cutting plaques for a university. We recently got a contract for all such awards for every organization within the university and due to the number of them needed a single fixture board won't fit the bill and honestly if I can get this concept to work this may turn into a full 4x8 fixture board and hold 21 or so at a time. The machining time is currently at 11 min per plaque but i'm working on toolpaths to reduce this. I have uploaded more pictures of the mdf after it was done. I did get some chipout & fuzz on the MDF but do not anticipate this once i switch over to my final material.
IMG_2849.jpgIMG_2850.jpg

[Jim Becker]

That's looking good, Adam. A quick hit with the ROS will get rid of the fuzz and if you seal all the areas "not under" the plaques on top as well as the sides and bottom, you should be able to use this for awhile with no issue to fully test the concept running multiple plaques. If you can use the Array Toolpath feature for all your common elements, (assuming your grid is dead-nuts spaced), it can minimize time hits from tool changes. You only need to manually do the toolpaths for personalization things, if there are any.

[Adam Bullington]

Jim,

All the current order will be a boiler plate design for all of them with only the name and number of the player changed on each one so each set of nine will be the same except for each of the names and numbers which i intend to save the file 9 at a time and move down the list of 74 and at the end I will have 8 separate files with 2 stragglers all in all i'm hoping it should work well but we will see. I am using the same file as i did for the vac fixture as the template for the plaque layout so everything should line up perfect..."emphasis on should" lol.

[Jim Becker]

Sounds good. So if you can use the Array Toolpath for all the common elements, that's going to save you uber-time because if can optimize tool usage. You then just need a file for each set that contains the personalizations. So that means one file for common elements and one file for each batch of personalized elements.

[Mark Bolton]

We do a bunch of plaques similar to this on a fixture with no vac (it only relies on the vac that comes through the MDF fixture from the spoil board). We dont do any edge profile on these so we just mill the pockets in the MDF to .750 and the plaques are about .800+/-. We cut the blanks on the slider but even with that there is very slight variation between them that can leave them loose or snug in the fixture. We deal with that with a wedge or cam on each pocket.

I would agree with brad that flatness of your parts is going to be critical with the gaskets. Even though we dont have gasketed pods in our fixtures we ditch the planer and wide sander all together and we just load raw blanks skip planed from the mill) and we fly cut the backs, flip, fly cut the front. If there are any pockets on the back for hanger/keyholes we do those at the same time. Fly cutting on the machine basically joints the back face and we setup a multiple toolpath that runs the first .020 on the back at a slow feed (blanks may be thick and thin/high spots) then a wide open .020 pass, then a finish .020 pass. 60 thou off the backs, flip, then two wide open .020 passes on the front and one slow. If you setup your pocket tool path for the deck off with a raster with the grain and no profile pass your parts (at least for us) are 150 grit and done. I dont miss standing at the planer and sander and I really dont miss having to grind out the scratch from the sander with lower grits.

We run the MDF fixtures for anything that is not going to be a daily deal or that we dont know for sure how long it will run. That way when the deal changes, we just toss it in the fire.

It will be interesting to hear how you like using the F4 to feed the pods. Also agree with brad that if you work the kinks out and go with another MDF option to paint your sheet all sides and edges first then machine your pods and you'll have tons of hold down. We are easily able to hold small parts with the F4 and where youve pocketed the blanks in the lateral will be zero. I will say again though that its always hit or miss for us to get large quantities of precise blanks off the slider. They are damn close but 5 thou here and there shows up in the blanks.

As Jim said, we just save our fixture drawing as the template for the array. We just drag it out of the clipart library and drop it in Vcarve. It has all the notes for the array right in the file. All toolpaths are on layers and have a toolpath template that we just load and go.

Congratulations, looks like a nice one!!

[Brad Shipton]

It seems you have a good plan. I am curious to hear how well the fixture works for your plaques. No points for prettiness for fixtures. Unless this will be a product line I would think about tossing this out when you are done like Mark suggests. It is easy to collect too many of these and never end up using them. That said, I have a container full of crap I keep that I will likely never use. haha

Keep in mind Jim does not have a tool changer. It will be important for him to final size before processing. The strategies for cutting parts is a bit different without a tool changer. I used 4 tools to cut out my face frames and about the same when I cut drawers. I am not sure how I would any of my parts in bulk without the tool changer.

Some food for thought in the future. Below you can see another fixture I use for making drawer parts. Here I oversize the blanks by at least 1/4" in all direction, and place them against the alignment pieces. When the part is final sized the cutter never touches the fixture surface nor the alignment pieces. The stock is only supported by the gasket material around the perimeter. I made 80parts with this and the largest drawer side was 5/8"x9.5"x30". The stock did not deflect more in the middle than around the outside and the vac I used for this generates up to 25" Hg. The common channel grid we use for our tables is a balance between maximizing the surface area between the parts you are cutting while leaving enough stock in place so your spoilboard stays flat. When you know exactly where the parts and cuts will be you can reduce the amount of support. More vacuum area between surface and part = greater hold down. Greater hold down = more resistance to lateral movement (lateral resistance is a function of friction, vertical force, and the stiffness of the gasket).

DTailJig.jpg

Let us know how it goes.

[Jim Becker]

Keep in mind Jim does not have a tool changer. It will be important for him to final size before processing. The strategies for cutting parts is a bit different without a tool changer. I used 4 tools to cut out my face frames and about the same when I cut drawers. I am not sure how I would any of my parts in bulk without the tool changer.

True, I do not have an ATC, but I do have an FTC (fast tool change...automatically measures length after the tool change pause) so I like to minimize those changes in favor of time savings and effort. That said, even with an ATC, if you can optimize the cutting to minimize changes, the job will run faster.

[Brad Shipton]

I know little of the FTC, but I will put that in the ol memory bank. 20-30s per tool change rarely impacts my cut speeds. For FF parts, 3/8" mortise bit, 1/8" mortise bit for corners, 1/4" roughing tool, and to save a bit of time sanding I use a final pass with a low helix cutter that leaves a nice clean surface. Drawers you have 3/8" bit for end pockets, 1/4" sizing pass, and the pins. Vortex suggests a 1/2" compression cutter but I do not have enough machine for that.

[Mark Bolton]

I hoestly think if you were sitting right there (which defeats the purpose of the machine to begin with) the FTC might be as fast as an ATC depending on where your working on a larger table. Tool changes in general are a time suck unless you have on-board tool change. We will often times fixture closer to the ATC to save time but it really only makes sense when your running 80 sheets a day and if you can shave 15 seconds off a sheet you gain 20 minutes a day.

I have recently begun to adopt a new philosophy (for me) in that Im looking at the total package. My shop is in a rural area, a lot of locals are self professed know-it-alls. They come into the shop and will watch a sheet of backs and bottoms get broken down on the CNC and think that they could do it just as fast (because they own a craftsman contractor TS and have cut a sheet or two of ply on their table saw). I always ask them "you wanna race?".

I can outcut the CNC on square parts on our slider. I can maybe run parts across the jointer and through the planer faster than I can deck them off 3 passes on the CNC. But the square parts I cut on the slider will be prone to error, mistakes, not square, trash inbetween the flip stop and the part, read the wrong side of the measure (37.5 instead of 38.5).. the planed parts will not be flat, and Im having to stand there grinding my old bones to powder the entire time.

Im recently adopting a mindset of not worrying about wringing every ounce of time out of the machine I can. I still optimize toolpaths meticulously, cut out wasted steps, but the sheer fact of letting the machine do what we would be shuffling and returning boards to the infeed operator to do is huge. And even running slower, throughput is higher, higher quality, and so on. It increases a 3 man shop to 5-6 in the pertinent operations.