|
Post by aquanub on Feb 7, 2020 23:42:43 GMT
Hey all, I've been running a power route for over a year now. For wood projects, its flawless and a complete beast. However when it comes to aluminum and other materials I seem to have an issue with achieving the surface finish I need. When cutting aluminum I run an air blast, so I know its not a chip evacuation / chip welding issue causing the surface to be rough. Perhaps this is a user issue... because I dont see very many other people complaining. I've been trying to accurately dial in the tram on this machine for months. I've watched almost every tramming video on youtube (I even machined out a pro-tram type tool at work to use), and I believe I have the machine dialed in to the best of its available adjustments.
This is the current tram I have obtained (measurements are across a ~19" span):
Left: -0.0005" Right: 0.001" Front 0.001" Rear: 0.003"
When I go to surface my material, I am still left with ridges I can feel with my finger: I've feel like I've tried everything. I've switched out the glass I trammed on in case of inaccuracies. I've tried running the facing op in various feeds / speeds / depths to no avail. I've checked every bolt for tightness. I've took apart and reassembled the Z carriage. I am about to redesign the Z carriage for better tramming adjustment, but I am not sure if it will alleviate my issues at this point. Anyone have any tips / input? Thanks!
|
|
oldtech
Full Member
Posts: 222
Machine: Power Route
|
Post by oldtech on Feb 8, 2020 1:20:06 GMT
I replaced the z-plate with a new wider plate coupled with a router mount plate. It is not perfect, but at least I can now tram without taking the rest of the z-axis apart and leave my dials in place while I tram.
What I would like are micro-adjustment screws for the traming.
|
|
|
Post by Bruce on Feb 8, 2020 6:45:02 GMT
I don't work with aluminum but the questions will be: What type of aluminum are you working with? And what kind of end mill tool are you using?
|
|
|
Post by aquanub on Feb 8, 2020 13:05:43 GMT
I replaced the z-plate with a new wider plate coupled with a router mount plate. It is not perfect, but at least I can now tram without taking the rest of the z-axis apart and leave my dials in place while I tram. What I would like are micro-adjustment screws for the traming. If you had some time could you share some photos? I would greatly appreciate it.
|
|
|
Post by aquanub on Feb 8, 2020 13:09:21 GMT
I don't work with aluminum but the questions will be: What type of aluminum are you working with? And what kind of end mill tool are you using? 6061 aluminum... nothing crazy. I know people with "lesser" hobbyist machines have no problems with it. I am well within the SFM of the material and I am using single flute carbide cutters. I've tried a wide variety of milling recipes to no success. Parts come out... but the tram or something else seems to be wonky .
|
|
agrpm
New Member
Posts: 32
|
Post by agrpm on Feb 8, 2020 17:09:19 GMT
There would still be several factors I would like to know to help narrow down your issue. Mainly, what is your programmed stepover for the Endmill your using? Judging by the toolpath "swirl" left behind it looks to be significant. Possibly in the 90% range? Do all the of steps tend to "lean" in the same direction? What depth of cut are you attempting to face off? Nothing extreme I'd bet, but still a valid question.
|
|
oldtech
Full Member
Posts: 222
Machine: Power Route
|
Post by oldtech on Feb 8, 2020 17:58:27 GMT
Here are some pictures (from fusion) of the zplate and its router mounting plate that I'm using. I should note that this design allows for moving the router/spindle up and down to provide more or less z-clearance. Note that the side holes in the zplate are threaded to make it easier to move the router mounting plate.
|
|
blinsc
New Member
Posts: 32
Machine: Power Route
|
Post by blinsc on Feb 9, 2020 15:26:48 GMT
I would recommend using a large (eg, 1") mortising bit with a 90% step-over and surface a piece of MDF. If it's nice and smooth, you know it's not a tram issue. Do this operation twice, once along X-axis and once along the Y-axis.
I've cut quite a lot of aluminum with my Power Route and my surface/pockets are always smooth to the touch using 1/8" and 1/4" end mills. I feel like if you're getting a ridge in aluminum, that seems like it's a mechanical problem, like an axis is flexing/binding.
I'm curious to know, in your first post/third picture - are the visible lines the ridges? And if they are, how were they originally oriented on the machine, and what's the spacing? If it's a tram issue, it should manifest itself as being the width of the step-over, but those ridges look pretty far apart, or you are using a large end mill. Can you tell us what type/size end mill you are using? While you may be within the SFM of the material, that is not really a good starting point for the Power Route. SFM is important but the specs posted by manufacturers are for big rigid mills, not small CNCs using woodworking routers.
|
|
|
Post by aquanub on Feb 10, 2020 1:00:41 GMT
I would recommend using a large (eg, 1") mortising bit with a 90% step-over and surface a piece of MDF. If it's nice and smooth, you know it's not a tram issue. Do this operation twice, once along X-axis and once along the Y-axis. I've cut quite a lot of aluminum with my Power Route and my surface/pockets are always smooth to the touch using 1/8" and 1/4" end mills. I feel like if you're getting a ridge in aluminum, that seems like it's a mechanical problem, like an axis is flexing/binding. I'm curious to know, in your first post/third picture - are the visible lines the ridges? And if they are, how were they originally oriented on the machine, and what's the spacing? If it's a tram issue, it should manifest itself as being the width of the step-over, but those ridges look pretty far apart, or you are using a large end mill. Can you tell us what type/size end mill you are using? While you may be within the SFM of the material, that is not really a good starting point for the Power Route. SFM is important but the specs posted by manufacturers are for big rigid mills, not small CNCs using woodworking routers. In the photos, the visible lines are indeed ridges. I can feel them when I run my fingernail over it. The toothpaths for the facing op are running in the Y direction. 1" surfacing bit with a 50% stepover. Depth of cut is .02". The spacing of the lines kind of baffles me as well. I've tried surfacing in just one direction (isntead of back and forth) thinking it was a material climb mill issue, but it didnt make a difference. I'm all ears for any suggestions as to what to check. When surfacing my wasteboard (the slats in the photos) I do not see any of these ridges. Thank you guys for your input thus far.
|
|
agrpm
New Member
Posts: 32
|
Post by agrpm on Feb 10, 2020 1:58:57 GMT
My gut feeling is that your having a deflection issue. Your creating a large amount of resistance against the tool using a 1" facing cutter on that aluminum. I recall reading somewhere that the routers and/or spindles most are using on machines this size do not handle postive force in Z+ against them very well. It's not the rest of the machine so much as the spindle or router that's creating your issue I would guess. I would cite several things in support of this theory. First, your able to surface softer material that would pose less resistance without any issues. Second, notice that Blinsc said he has had no issues cutting aluminum with 1/8" or 1/4" endmills. The surface contact of those tools against the material VS what your attempting to use is drastically different. And 3rd, provided you are sure that everything is taunt and secure on your gantry, your tram looks great.
Humor me and try the same toolpath with a .25 endmill with that same 50% stepover.
|
|
blinsc
New Member
Posts: 32
Machine: Power Route
|
Post by blinsc on Feb 10, 2020 4:48:16 GMT
I get the sense that agrpm is right about the deflection. I never use larger than 1/4" in aluminum, mainly because the DW618 starts to bog unless I back way off on the depth of cut, but I could see deflection of the machine being an issue as well with a 1" bit. Plus a bit that big is going to want a low-ish RPM and the DW618 (like any other router) to drop in power if you go too low (eg, under 14k RPM).
Derek - if you see this, can you recommend the largest surfacing bit/depth of cut for the Power Route in aluminum?
|
|
|
Post by Derek the Admin on Feb 10, 2020 5:11:56 GMT
I don't have a specific recommendation on the face mill size, but I personally would not run a 1" face mill on aluminum with it. Furthermore, the rake angle impacts the forces as well. Adding more to this, it can be as simple as the bed just shaking. We run a big (3", 7 insert) face mill over some aluminum parts and just a little bit of overhang from a vise edge, even with a relatively thick piece, will leave significant swirls on the part. I know you aren't cutting over a vise, but facing metals with a big diameter mill is a high force endeavor.
Lastly, a 1 inch mill even running at the bottom of the 618's range is at about 2100 surface feet per minute. I personally wouldn't run that surface speed in aluminum without a high end coated carbide insert or end mill and flood coolant.
|
|
|
Post by aquanub on Feb 10, 2020 13:41:28 GMT
I don't have a specific recommendation on the face mill size, but I personally would not run a 1" face mill on aluminum with it. Furthermore, the rake angle impacts the forces as well. Adding more to this, it can be as simple as the bed just shaking. We run a big (3", 7 insert) face mill over some aluminum parts and just a little bit of overhang from a vise edge, even with a relatively thick piece, will leave significant swirls on the part. I know you aren't cutting over a vise, but facing metals with a big diameter mill is a high force endeavor. Lastly, a 1 inch mill even running at the bottom of the 618's range is at about 2100 surface feet per minute. I personally wouldn't run that surface speed in aluminum without a high end coated carbide insert or end mill and flood coolant. I should have clarified, the 3rd picture posted is not aluminum. It is acetal, surfaced at 40ipm and a DOC of 0.01" or 0.02" I havent bothered trying to surface aluminum if I can't get it proper on a much softer material.
I know the best way to surface this material is with a flycutter at very low RPM's but the lowest the 618 can run is 8krpm.
Perhaps I need to go to a spindle with VFD?
|
|
|
Post by aquanub on Feb 10, 2020 13:46:59 GMT
My gut feeling is that your having a deflection issue. Your creating a large amount of resistance against the tool using a 1" facing cutter on that aluminum. I recall reading somewhere that the routers and/or spindles most are using on machines this size do not handle postive force in Z+ against them very well. It's not the rest of the machine so much as the spindle or router that's creating your issue I would guess. I would cite several things in support of this theory. First, your able to surface softer material that would pose less resistance without any issues. Second, notice that Blinsc said he has had no issues cutting aluminum with 1/8" or 1/4" endmills. The surface contact of those tools against the material VS what your attempting to use is drastically different. And 3rd, provided you are sure that everything is taunt and secure on your gantry, your tram looks great. Humor me and try the same toolpath with a .25 endmill with that same 50% stepover.
Here it is with a 2FL .25 endmill, should have probably fed it a little slower but similar ridges are present.
|
|
jms
Full Member
Posts: 168
|
Post by jms on Feb 10, 2020 13:50:43 GMT
I haven't face milled aluminum yet on cnc, but I know on my millrite milling machine, I use a HSS fly cutter, rpm is less than 1000, and I only take .003 at a time. comes out like a mirror. 20 thousands is too much.
|
|