hi team : HOW I CAN DO IT BY sketchucam ? i am sorry because my English language weak so i hope someone understand my issue ! i work on sketchucam , i have piece of aluminum ( for ex: 10cm*10cm*2cm high). i want the cnc to eat each side 2mm (to be squared ) all sides . the problem it is that the sketchucam work only on z axis to cut , i mean it cut from up to down only. but i want the cut from side to side like as the pictures show ! ( i want the cut from side to side ,not from plunge . i have end mill 4 flute so i want to use it for cut the sides may be this video explain my needed : or this : HOW I CAN DO IT BY sketchucam ?
i try with inside cut and with outside cut and with boundary cut but not work i want multi side cut (side by side ) instead plunge multi cut!
SketchUcam has no knowledge of the outside of the final piece since it is designed around cutting shapes from a large sheet of flat stock. (see 'Phlatprinter' on youtube) so, my method for squaring your bit of stock..... Draw the rectangle of the final size you want. draw a larger rectangle around it (leaving some extra space beyond your stock, depending on your bit size) 'pocket FLOOD' the space between. delete the outer rectangle cut. group the zigzags together so they cut first. I found it better to rotate the rectangles 45 degrees before pocketing. then rotate them back. This gives a safer zigzag cut that will not cut a full depth cut along an edge since it is all at an angle to hte edges. Remember to turn on RAMPing and set the right angle when cutting aluminum.
thanks David is this cut from side to side or from up to down ? i mean : did you see the second video at 00:49 ? the end mill not plunge from up to down in the piece , it is cut from side to side . * you mention me about ramping in z ! the ramping i used when i plunge at the surface of the piece only (not at sides i think) could you please make video to explain how cut the sides of stock by sketchucam
Did you download the file I posted and run the gcode? Use a 6mm bit and cut a piece of insulation foam, then you will see what it does and gain understanding. Sketchucam does not do cuts like those shown in the video. Those are called HSM paths. If you really need those, and have a 10horse power mill that can do it, then maybe you need Fusion360? In Sketchucam You could draw lines by hand and then set them as centerline cuts, then do a finishing pass with an outside cut. This is tricky to get right. Meanwhile, please watch these videos and read the manual so you can better understand this tool... Phlatboyz SketchUcam Help
Did you download the file I posted and run the gcode? *not yet ...but i will do it soon. Sketchucam does not do cuts like those shown in the video. Those are called HSM paths. If you really need those, and have a 10horse power mill that can do it, then maybe you need Fusion360? In Sketchucam You could draw lines by hand and then set them as centerline cuts, then do a finishing pass with an outside cut. This is tricky to get right. yes ...that's what i want to know ...i have to do some modification to do some cuts because the sketchucam not support it.) am i right? i red all help and watched all video on you tube ....and test them all so i start to get some experience too ...but i ask to make sure of some wondering. ********************************************************************************************************************************************************************* now about spindle power : my spindle has 1.5kw ...i know it is not good for some cuts ..but all i want it is to cut just 1mm from side ...i think i do nor need 10hp to cut just 1mm from side why i need to cut from side instead plunge with end mill ? ..because i have None center cutting endmills. so i can not cut from up. please correct my answer if i am wrong !! thanks David
other question : how control the cuts direction or cut start point ? please see my small example : see the picture : i draw rectangle and made 4 offset with 2 distance between them ...so the outer rectangle No. (1) its is the true size of my piece the fourth rectangle (4) it is the final size i want ( my objective ) the second and the third it is just steps to reach my final shape NOW ... i made outside cut tool for all rectangles . the problem it is that the toolpath start from inside rectangle , not from out side how i can change the start cut to be from outside to inside ?
You could just make four separate g code files and run the outside one first, then work your way in to the final size by running each file. Or make them separately then join them to run as one file.
how i can change the direction of cut ? to do (climbing cut) ......i think the sketchucam are weak to make some professional cuts. ( may i am in wrong ) but i still learning. please guys be patient with me
RAMPING solves this! SketchUcam: HOWTO use Ramping There are situations where it cannot ramp and will convert to a plunge (when the line segment is too short). There is always a warning comment in the Gcode when this happens, so you just need to read the Gcode and check for warnings. Code: G00 Z5.000 X12.278 Y10.566 G01 Z-6.300 F1000 (ramplimit end, translated to plunge) X12.060 Y11.045 F2000 X11.454 Y12.123 The line just before that warning shows that it is plunging down to -6.3mm, you have to prevent that. The optimizer does search for a long enough segment for the ramp and will only plunge if one cannot be found. If your shape does not have any long segments then you will have to pre-drill a hole for the tool to enter (using a real drill bit of course). What is long enough to ramp? A segment must be longer than the bit radius. This allows for tools where the end cutting edge is larger than half the radius to be ramped. If the cutting edge is smaller than half the radius, then it will get jammed on such a short segment. To force a cut to start at a desired place you can place a plunge hole near the start point you want, then group the hole and the cutline. Why does this work? Because groups cut in group order. The plunge hole is a group. So when it is grouped together with another cutline, the hole will cut first, then the cutline. The optimizer starts the cut at the closest point to the last cut end point. But, you don't want a hole, so make it 1% deep. 1% of 10mm thick material is 0.1mm. If that makes too much of a mark, you can search and replace that depth in the Gcode to prevent any tool touch.
hard to help you more until you have studied that file and run that code. You can simulate the Gcode with this CAMotics so you can see where the tool is moving without running the actual machine, but I still prefer the 'cut some insulation foam' method (-:
To do the cut shown in the video, you probably need more power. This is because it is cutting about 30mm deep in one pass. Even though the side to side cut depth is very small, 30mm of tool engagement takes a lot of power (and a stiff, heavy machine). So, 1.5kw means you cannot do a cut exactly like the one in the video, but you will be able to do it in multipass layers. What machine do you have?
thanks David the conversation with you gave me more experience my machine (diy) i build it on my own see picture.
about the g-code ....i ran the g-code ..... do you mean the endmill will cut the side by zigzag ? the end mill eats the side with same way you draw zig zag ...i think finally understood your way again : see the picture please : No 1 means the cut done No 0 means the cut not done the edge of the piece become some cut and other not cut because it follow the zigzag line as in picture so we need the boundary line to cut the rest of zigzag ... all the way ...thank you very much M.Savid you gave me many ideas to go ...so i will try your way and i will edit it to cut in good way ...
well, I don't know what you are doing. The cuts I drew will do: the zigzag to remove most of the material from the edge then a final cut to clean the surface the zigzag is purple the final cut is blue (because I selected it to highlight it) That is a continuous straight line cut all the way around the part to clean the edge. (and it can be seen in your picture!) so there are 2 cuts. If you only got a zigzag, then you must have selected it before generating Gcode. You should get 2 cuts and a clean edge. Make sure you have nothing selected when you generate the Gcode.
yes ...exactly ..that what i meant ( but i could not explain it with English exactly).....it is works good . cause of your help , i found other way ..it is very easy and new ( i think no one know it ) i will post the new way here ....just after make some test . thanks thanks thanks ...all my issue finished.
David the swarfer finally...i control on the path tool ...now the end mill can start from outside and goes to inside edges ( one by one) pleas run the g-code in attachment inCAMotics and see the toolpath . the inner shape it is the final shape and the outer it is the new piece that i want to machine it . so i can also make the end mill start from inner to outer . did I make discover or no thing is new ? if that is new for the builders , i will explain my way ! and i hope put your comment about this note : this way without join multi code files...just one run
Both your files have warnings in them and the Gcode is not really valid. Code: G90 G21 G49 G17 G61 F2540 M3 S15000 (RETRACT limiting Z to @max_z) <---- this is a problem! G00 Z0.000 (RETRACT limiting Z to @max_z) Z0.000 G01 X105.054 Y312.356 F6500 Z-3.000 F2540 X415.054 F6500 Y622.356 X105.054 Y312.356 (RETRACT limiting Z to @max_z) G00 Z0.000 G01 X106.054 Y313.356 Z-3.000 F2540 (RETRACT limiting Z to @max_z) is a warning that you have not correctly set your MAX_Z value or are using material thickness + safe height that is too high. However, I believe it is set to 0 which is WRONG, MAX_Z must be set to the distance your Z can travel otherwise it cannot lift to a safe height above the work (since the work surface is Z=0). MIN_Z must be negative Z travel to allow it to travel below the work surface. Urgently go and read this SketchUcam - Thing to do After Instal and fix your settings! Note that the Min_z and Max_z settings are not foolproof in preventing machine crashes. If you are machining thick parts you need to think about the clearance and Z travel limits.
ohh... i forget to tell you that i have 2 pc ....one in workshop that connect with cnc ....and other in my flat ( that i write from it to you now ) this pc ( sketchucam) not correctly setting and just for test some generate g-code ........ i mean , do not care about these warning .
