- March 13, 2017 at 3:47 am #29316
Hi gang, I designed a piece that was being cut out of 5/8mdf and I added some wording on the surface that was 2D contoured to 1/16″ depth. The feed rate was set to 1100mm/min. This was done in Fusion 360 and loaded in Repetier.
When I run the job, the cutting out of the part is good, but the lettering is super slow on any part of the letters that’s not a straight line. The straight parts are at speed, but the remainder are super slow. Microscopically slow.
How do you fix it ? Any ideas ?March 13, 2017 at 5:15 am #29320
In gcode, arcs use G02 and G03.
You should look at the gcode, look for G02/G03 and see if the First is set right. Maybe the postprocessor isn’t handling the unit conversion correctly.
Are there other kinds of curves that are that slow, or just the letters?
Microscopic slow sounds like a mm/s is being used for mm/min.
IIRC, the EstlCAM tutorial has you configure it to not use G02/G03, which makes it replace arcs with a bunch of lines. I don’t remember why that is though.March 13, 2017 at 5:17 am #29321
There are some rounded corners that are displaying choppy speeds (not fluid through the corner). Thanks. I’ll check it out tonight.March 13, 2017 at 5:27 am #29324
Which fusion360 posts processor are you ussing? My implementation (https://github.com/martindb/mpcnc_posts_processor) use arcs (G2/G3), but only if the arcs are big enough. Small curves are just plain G1.
Please post your GCODE file.March 13, 2017 at 5:42 am #29326
Yes yours. Will check it out tonight and post gcode.March 13, 2017 at 12:01 pm #29354March 13, 2017 at 12:20 pm #29357
Indeed, those are all G1 movements. The feedrate looks reasonable, most are 1100, although some are 2000, some are 762, and some are 400.
There are some movements that are x, y, and z at the same time, Marlin will limit the speed along the path so that each axis will not exceed it’s own speed/accel/jerk limits. Is it possible that’s what’s causing it to be super slow?
I am attaching a smaller version, with most of the F1100 stuff removed (grep -C1 -v “F1100”, for Linux nerds.)
Attachments:March 13, 2017 at 12:23 pm #29359
Jeff that is the problem, Marlin doesn’t always limit it.
Sometimes it will reboot, sometimes it will try to move at the wrong speed, rarely does it limit the speed. I don’t know enough to figure out why it happens. I think marlin might limit it if it is one axis at a time but seems to not do the math if it is multiple axis at once.March 13, 2017 at 12:51 pm #29361
Is that with a specific firmware version? @P3DCNC, what version are you using?March 13, 2017 at 12:51 pm #29362
It seems like all 2.5D cutting would require 3D movements. Why isn’t this a more common problem?March 13, 2017 at 12:54 pm #29363
It was more common, that is why Christian changed Estlcam, and we all updated the fusion post processor.March 13, 2017 at 2:17 pm #29368
I’m using RC7.March 13, 2017 at 4:18 pm #29374
I’m also using the v10 post processor “MPCNC_Fusion360_V10_SDcard.cps”.
Are RC7 and V10 the combination I should be using ?
Here are the speeds in Fusion. So that’s where the 1100 and 762 come from.
Attachments:March 13, 2017 at 4:33 pm #29376
762 is too fast, that is 12.7mm/s faster than the axis max speed of 8.5mm/s or 492mm/min. The suggested is 3-4mm/s.March 14, 2017 at 6:08 pm #29530
Your uploaded gcode was not generated with my posts processor version. If you try my version, gcode file should be smaller, because the G2/G3 (aka arcs) use.March 15, 2017 at 3:23 am #29556
Ya, I thought it was the same thing. I now realize that there are different streams of post processors floating around. The one I was using is the one I listed above “MPCNC_Fusion360_V10_SDcard.cps”. I’ve downloaded yours and will give it a go.
Maybe we can consolidate these to a common recommended one ? To minimize confusion.
Thanks.March 15, 2017 at 3:27 am #29557
I still would like to know if others have to add tolerances to jobs like this. Just to know if this is normal or I have something going on in my setup that shouldn’t be. Thanks.March 15, 2017 at 8:24 am #29580
I have consolidated them to some recommended ones. https://www.vicious1.com/software-updates/ they have branched off so now we have options.
Tolerances will differ per machine, exact fit is almost never recommended. I suggest just making a test part something small. try a few different settings and then you will now about how much to use after that in that material. All part of the fun.March 16, 2017 at 11:55 pm #29686
I’m going to start a new thread about the post processors. Definitely something funky with V10, and Martin’s has some issues as well…March 17, 2017 at 7:10 am #29702
Bummer. I made a bunch of cuts with V9 and it worked great so go with that and I will try and figure out what changed in V10.
You must be logged in to reply to this topic.