Why can't I cut a simple pocket with a 1/4" EM?

1

Shapoeko 3 XXL with compact Dewalt router and Z-belt drive. Using a 1/4" compression bit.

Trying to cut simple pockets in the attached file but the router cannot complete the first pocket without thumping and bumping which completely throws off the z-height for the rest of the pockets.

I have had this problem before when just trying to cut the through holes for the spoilboard. It was suggested that I use a 1/8" bit instead which does seem to work better for the wasteboard holes which are a 1/4". The pockets in this file are much larger than the 1/4" bit I am using so I do not understand why this machine is having such an issue with basic pocket holes.

I am taking 1/8" deep passes in 3/4" MDF and it still cannot complete the first pocket without basically crashing and throwing off the Z height.

Any suggestions for fixing this would be much appreciated as it has been a problem since I got the machine.

Paws Hearts.c2d (220 KB)

Kind Regards,
Bryan M.

2

A Compression bit wants to be deep enough in the material that the upcut portion is fully engaged and at least part of the upcut geometry is cutting — not an easy thing to do an a belt-drive machine.

A further consideration is you are cutting quite thick stock:

image
image666Ă—1287 21.6 KB

My recommendation would be to instead use a pair of tools:

  • downcut along the perimeters of the cuts to establish a nice edge:

image
image804Ă—825 15.9 KB

Note that the suggested Depth per Pass here is 0.060", less than half what you were trying

image
image2880Ă—1728 459 KB

Then, change the tool to a #201 upcut — this will help in chip clearing, always a problem in MDF, and yield a nice cut at the bottom:

image
image2880Ă—1728 412 KB

Note that you will want to be very careful of the zero since this cut is right at the flute length of the tool — if you’re deeper than the machine thinks you should be you will get rubbing at the top of the tool.

  • probably for the perimeter you should do the same thing, so offset the outside geometry by endmill diameter plus 10%:

image
image2880Ă—1728 378 KB

image
image2880Ă—1728 340 KB

Then set up a pocket to cut the outside down to tab height:

image
image2880Ă—1728 421 KB

image
image2880Ă—1728 434 KB

and it will preview as:

image
image1920Ă—1152 160 KB

and should cut well:

Paws Hearts_v7.c2d (236 KB)

3

A belt drive SO3 would have a hard time cutting a 1/8" DOC. Of course you could upgrade to a Z-Plus or an HDZ but even those two might not be able to get 1/8" DOC in MDF. MDF is surprisingly hard to machine. It is glue and saw dust and is tough on tools and machines. Frankly an SO3 is a good machine but it has limitations being a belt drive on all 3 axis. I have an SO3 XXL with HDZ and love it. However the belt drive Z will work but you cannot push it too hard or it will miss steps and get your Z zero off. As @WillAdams stated compression bits are designed to take full depth cuts in plywood and will not do that on an SO3. The advantage of a compression bit is it is both up cut and down cut but that only works with a full depth cut. I think you might be better off with a down cut bit that is just a straight end mill. The compression bits work well on industrial machines with a lot more rigidity and power but not so much for an SO3.

1 Like
4

Thank you both for the great tips and advice. I have changed my file to follow the suggestions from Will and doing some more tests. The MDF is merely for testing before I cut a actual hardwood.

Hoping to upgrade to the HDZ and then a spindle one day but need to get some project sales under my belt to get there.

Thanks again guys. I will post some pics of the completed project once everything is worked out.

2 Likes
5

Well we can’t celebrate just yet. It is still having the same issue when attempting to cut the first pocket with the upcut using the suggested method that Will recommended.

This machine just does not like to cut deep pockets with a 1/4" end mill. Downcut or upcut.

Could this be caused by an overtightened belt on the Z?

Might be time to get rid of this belt drive Z and upgrade to the HDZ sooner than later.

Regards,
Bryan

6

What is your depth per pass?

Is the tool sharp?

7

Depth per pass is 0.060 and the 201 end mill is brand new.

The downcut is cutting to 0.125 in 0.060/pass increments. But the problem occurs when it tries to cut the rest of the pocket below the 0.125 depth left from the downcut.

I also have the toolpath set to ramp in at 20 degrees. Plunge rate is 15. Feed rate is 75 ipm.

Should I slow this down because of the limitations of this Z-Belt?

Is this a possible belt problem?

Regards,
Bryan M.

8

Belt tension needs to be guitar string tight on the Z-axis.

9

Ok. It seems to be within that tolerance.

I may consider order a new belt for now. I bought this machine used from a gentleman that had it for over four years but never used it. I have been using it heavily for the past 6 months so maybe the belt is weakend from sitting for so long and then getting used heavily.

Otherwise, I will look into upgrading to the HDZ in the near future.

Thanks Will.

Regards,
Bryan

10

My belts are from 2016. They are still good. I did replace my belt Z with an HDZ but the belt on that was still good. If you suspect the belt then take it off and turn it inside out and inspect it for any missing or deformed teeth. Same for your X and Y belts but you can likely just turn them over on the machine and inspect them. The original belts were gates fiberglass reinforced belts. Later they went to steel belted ones and there were a failure. They would get distorted and looked like the teeth had been stretched. If you have the steel belts you can likely put a magnet on t hem to see if it is attracted.

Something else is wrong likely. The machine tries to go to the depth you specify and with a belt Z you could be losing steps. That usually results in a deeper pocket than you wanted. I have cut many pockets with an upcut or down cut on my SO3 and they always cut accurately.

Be sure to check the lower v-wheels. With the SO3 powered off push on each one and you should be able to just move the Z axis and/or the gantry. If the wheel slips then you must tighten the eccentric. To do that you loosen the bolt with a hex wrench and use a wrench to turn the eccentric. Then when it is tight you hold the wrench on the eccentric and tighten the bolt. Failing to hold the eccentric with the wrench can cause the v-wheel to be over tightened. If the Z is flopping around due to loose v-wheels you will get varying depth due to deflection of the Z. The v-wheels on the top of the Z and X and Y are not adjustable but should be clean and able to rotate freely. To check that you need to loosen the bottom v-wheels to get enough slack to rotate the top v-wheels freely and to inspect them for flat or broken spots. Loosening the eccentrics would require you to readjust them as above.

Lastly how deep are you seating the Bit in the collet. The collet is around .75" long. So for the best grip on the bit it should go in at least to the top of the collet. It can go higher but never push the bit all the way up in the router shaft. The top of the router shaft is rough and when the collet is tightened it slightly moves the collet and bit up an inclined plane. If the bit is all the way up to the top it has no where to go and can become loose and slip during cutting. If you seat your bit too deeply is it possible the collet nut is rubbing on the material top.

2 Likes
11

Hey Guy. Thank you for your response. I have tried to adjust the v-wheels on the Z and believe they are properly adjusted but I am still having the issue. It starts cutting the pocket and about 1/3 to 1/2 way into the pocket I hear the machine “thump” as if it bottoms out. At that point the depth of the pocket and remaining pockets are not correct.

I am actually cutting a through pocket so the depth of cut is stock bottom but it never gets that far,

I am inserting the bit to the top of the collet as has been suggested by others. So there is plenty of room between the top of the bit and the router shaft.

At this point I am stumped about what to do to fix this problem. It has been a consistent problem since I got the machine. I have adjusted the belt on the Z and all of the v-wheels that can be adjusted but I still cannot cut a pocket deeper than 3/8" to 1/2".

If you or anyone else has any ideas I would appreciate any advice or suggestions about what to try next.

Kind Regards,
Bryan M.

12

If you have the belt drive the thump is the Z missing steps. I suggest you take the Z off. You take the bottom v-wheels off and the Z will pull out at the bottom and come off the gantry rail. Unplug your electrical connections and from behind the belt Z you can inspect the belt for missing or marred teeth. You can more easily adjust the belt tension.

Just make sure you are using the default F&S for the tools you are using because the belt Z cannot take big bites. With the Z off and laying the table you can remove the belt and inspect it and put it back on and adjust it.

The v-wheels have a small washer between the v-wheel and the frame. Make sure those are in place otherwise the v-wheels will rub against the frame and slow down the X motion.

13

That’s too fast for feed rate for that machine. I’d start at 35 ipm and go up to 70, but consider this next item.

Have you checked to see if your Z movement is bottoming out before the end of the bit is? Or even if your “safe Z” is set too high? Either one of these can cause the Z to “grind” and lose steps.

EDITED SPELLING

1 Like
14

Is the router mounted to high in the router mount and physically unable to lower enough without losing Z steps?

1 Like
15

I have a suggestion that might help with a little back story as well.

Try using a small drill bit that can cut a relief hole prior to milling the pocket, that is, if the pocket is something like a hole. By removing the center of the pocket with a drill takes away added stress to the endmill when plunging into a hole.

I have had these some problems while machining metal in the machine shop. To fix this issue, I would run a smaller relief cut into the hole and then follow it with the desired diameter cutter.

The problem it sounds like to me is that the feed is one of the problems. If this is the case, just slow it down a bit to see if that works. Even cutting the feedrate down by 50% would give you an idea if it is enough. Also, length of endmills do play a role if the tool is long sticking out of the collet. The further out it is the more likely you will have tool deflection.

In a plunge cut, deflection can become exaggerated because of the pressures that are pushed upon the tip of the endmill. If you are cutting the small pocket where the endmill is not moving that far from the centerline of the hole, then material buildup can be a problem. I know you tried different types of cutters and they still didnt work.

With a belt driven machine, you say you have heard the thud as if the machine has bottomed out, that sounds like a belt jumping teeth. You checked all belts and V guides and say they are good. So, the only other thing is possible is that you are pushing the machine too hard and the return force against the drive motors as the machine tries to cut compounds the faster, or deeper you go into the cut per pass.

I know this is a bit long winded, but I would be reducing the feed of my machine and/or running a relief cut moving forward. By process of elimination, you should have found the problem if it was in the machine’s hardware, (belts, guides, motors, spindle collets, etc.). Now if its not any of these, then you look into the program, (depth of cut, type of cut, feed rates, spindle speeds, etc.).

Hope you figure this out and you touch base back with us to give us the good news of it being fixed and what the issue was. Good luck.

1 Like
16

This topic was automatically closed after 30 days. New replies are no longer allowed.