I want to mill steel with this machine.

More
04 Jun 2020 11:25 #170093 by Aciera
Only possible way I see is to use a high speed cutting strategy. Some CAMs have that option bullt in:

Looking at your z axis set up and how far out your spindle is mounted I doubt if your machine is really rigid enough to handle the forces. And then there is the issue with the hardened edges from the plasma cutter. I know people with real machines like the one in the above video who will not mill into a plasma cut edge. So If you really want to mill steel on your router you might be better off milling the holes all the way.
The following user(s) said Thank You: tommylight

Please Log in or Create an account to join the conversation.

More
04 Jun 2020 19:07 - 04 Jun 2020 19:13 #170120 by machinedude
even with that video if you pay attention at one point the tip of the cutter is red hot and tossing sparks. the video is not straight through so in those breaks i know the tool is being swapped out for a new one before the finish pass is done and possibly during roughing as well.

when you get into high speed machining your tools and holders have to be balanced to run at those speeds. they do often run with just air in these applications because coolant would trow the tool into thermal shock. in the video with a VMC those DOC. are really light and they don't look like more than .005 to .010 deep (imperial)

i still think spindle speed or lack of lower ranges of speed is the thing that will hinder cutting steel the most. feed mills work well with harder material with the right inserts but i doubt spending $200 on a holder and another $100 on a box of inserts is that attractive to most. the down side to those kinds of cutters are the are not flat bottom cutters so they don't get all the way through the part unless you have the clearance to do so in the set up.

because the edges are plasma cut most likely that will need slower speeds as well just because of that part of the plan.for the whole plan to be cost effective the tooling needs to last somewhat. with carbide if the rigidity is not there in the machine you will find out fast enough. carbide is great but it loves rigidity. so if the rigidity is not there tooling will chip or break pretty easily.

i have worked with all types of burn outs over the years they are tough no matter what tooling or machine you use. so being able to adjust things to get the job done is important. when you loose the ability to slow things down speed wise the task is even harder yet.

this is all just my 2 cents since this is what i deal with in my trade.
Last edit: 04 Jun 2020 19:13 by machinedude.

Please Log in or Create an account to join the conversation.

More
04 Jun 2020 23:23 - 04 Jun 2020 23:37 #170171 by Marcodi
All the tools I have are carbide. I don't have a single HSS tool laying around.

I am working in solidcam so yes HSM machining can be choosen.
I have coolingwater on the machine aswell. I looked at this video, but that is insanely fast, that could never go well with my machine. + The smoothness of motion I could also never reach in linuxcnc , it will give jerks or points where it slows. I posted a topic on this aswell a week or 2 ago and the conclusion was that linuxcnc can't do better because of lacking S curve acceleration and things like that. I had the issue that doing helix entries after every full circle it kind of halts/jerks before moving to the next circle with settings g64 p0.1 q0.1 which is my standard setting through all gcode.

Is it not so that the tool would simply break before anything else would happen to the machine or motors/carriages/guide rails.

I am used to always run above 12000rpm on the spindle. I don't really know how much power is in the lower rpm regions. Never needed to as it's always carbide tools. I know drilling has never been a problem at low feeds only drilling on my machine vises has been an impossible talk as that is a special hardened outer rim which is the hell to go through. But that's only downward action.

I use gwizard for feeds and speed in aluminium and solidcam 2d machining which complete chooses all settings for the cut after choosing what material I am working in. Only used it for aluminium and works like a charm.

On the other hand with a 160a power on the plasma on 12mm mild steel. How accurate would it be possible to make 16mm holes?
Last edit: 04 Jun 2020 23:37 by Marcodi.

Please Log in or Create an account to join the conversation.

More
04 Jun 2020 23:34 #170175 by tommylight

On the other hand with a 160a power on the plasma on 12mm mild steel. How accurate would it be possible to make 16mm holes?

Depends on a lot of things, but, around 1mm with some practice, 0.1 to 0.2 with lots and lost of practice but might not be possible due to nozzle/torch/air humidity/material/some fuzzy stuff that happens to plasma during cutting.
Rod and thefabricator might be much more helpful with this as they do some very nice holes on thick material, all i get is some oval..... so i do not bother with anything under 30mm in diameter even on thin material.

Please Log in or Create an account to join the conversation.

More
05 Jun 2020 00:11 - 05 Jun 2020 00:16 #170183 by machinedude
carbide has different grades the lower end carbide i think has a hardness of around 65 hrc and the higher end carbide has a hardness around 85 hrc. coatings on the tools can help with tougher material too.

i think with material 12 mm think you might get a hole kinda round but tapper is going to be hard to avoid with the hole sizes no matter what you do on thicker material. plasma is not exactly a precision process in my opinion.

12,000 rpm is pretty fast for steel. if you can get down to 8,000 or less you might have a chance but that's still pretty fast and you are going to be limited to small diameter tools at the speed.
Last edit: 05 Jun 2020 00:16 by machinedude. Reason: more information

Please Log in or Create an account to join the conversation.

More
05 Jun 2020 12:41 #170249 by andypugh

I did say it is possible, and the rest seem to forget you are talking about routing on already plasma cut parts,


I wonder if it might be better to cut the holes with the milling cutter. Perhaps pre-cutting with plasma is not helpful?

Can you swap the spindle temporarily? The best way to cut the holes is probably with an annular cutter (as used by magnetic drills) without pre-cutting with plasma. If you could buy / rent a mag drill and mount it to the gantry, then the job would go fast and clean.
The following user(s) said Thank You: tommylight

Please Log in or Create an account to join the conversation.

More
05 Jun 2020 13:28 #170252 by tommylight
Someone else also suggested drilling them with the router, as it is a better solution, but by far the best solution is Andy's drills, they are magnificent.

Please Log in or Create an account to join the conversation.

More
05 Jun 2020 22:49 #170293 by Marcodi
@andy, yes I actually could take out the mill and I have a magcutter here. Have to make something to fit it but that's not a issue.

Is that dirll would be within 0.1 that would do the work indeed.

Still have to do the outside profile of the plate but if I would run that at 0.1mm per pass. It's only 12mm total, that wouldn't be a too lengthy job. I could use a 6mm 4flange cutter running it with coolant

That seems indeed a good idea, as long as this angular cuttur ( I believe as to what you mean is a hollow kind of mill/drill.) Is accurate enough

Please Log in or Create an account to join the conversation.

More
06 Jun 2020 12:00 #170353 by tecno
Do you have anyone laser cutting close to you?

Please Log in or Create an account to join the conversation.

More
06 Jun 2020 18:38 #170384 by Marcodi
I have but they are just asking so much money for any work.

Please Log in or Create an account to join the conversation.

Moderators: cncbasher
Time to create page: 0.219 seconds
Powered by Kunena Forum