Help with a Quick G1530 CNC Router

[Kevin Flowers]

David
i have a chinese router that i purchased second hand, does everything i need it to and your one looks to be of higher specification. Mine doesn’t have vacuum hold down and if you are going to do acrylic or rout trays etc it is needed.
DSP controller is very easy to use, it basically takes a gcode file via thumb drive and allows you to set speed, travel etc although subject to the manufacture they can be programmed to do a lot more things. You will need a program to create the gcode i would recommend something like Cut 2D from Vectric they do a range of other programs if you want 3D etc http://www.vectric.com/ If you need any more info please get in touch

Kev

[Martin Pearson]

Think you will find the general feeling people have about Chinese routers is aimed more at the entry level machines David rather than machines like this one.
Is it just the router or does it come with a computer & software?
What software you buy for creating gcode will depend on what you want to do with it but as Kevin says cut2 D will be ok for stuff like flat cut letters & sign trays.

Kevin what Acrylic & tray work can’t you do with out a vac bed?

My machine is still pretty new to me although the actual machine itself is probably 20 odd years old or more. Have test cut quite a few different materials & didn’t seem to have a problem cutting acrylic & using tabs to hold bits in place.

[Kevin Flowers]

Martin
problems arise when cutting from full sheets you cannot clamp it in the right places or enough places so you get chatter on acrylic with the trays as you cut, it wants to lift so you get uneven depth of cut. You can eliminate it but by the time all the clamps are on to keep it flat the little palm router i have has done the job

Kev

[Martin Pearson]

Are right, not tried cutting from a full sheet, just smallish bits, my table isn’t big enough to fit a full sheet on although I should be able to cut a full sheet using tiling.
Take it you have tried downcut bits to try & stop the material lifting.

[David McDonald]

Hi Kev

Thanks for the reply, I’ll take a look at the software. Do you have any user instructions of any type on the DSP? I know they will be different brands but I’m sure there will be some similarities

Cheers
Macky

[Kevin Flowers]

David
may have a PDF at the workshop will have a look but if you go on to You tube and search DSP Pendant Controller you will get loads of Vids come up. It is very easy to use and the better programmed versions allow adjustments whilst running etc. It allows the machine to be totally independent of a computer allowing restart from a certain point in the Gcode after a bit break, power out etc, soft start for small bits etc. Vectric software is good, take a Vector file and assign a tool to the path as in depth, bit size. It does give you option of speed control but as said most pendants control that, then save to thumb drive. You may find that it will come with a program called UCanCam which is a Chinese gcode program never used it but been told it is glitchy. If you need any gcode files sent down to try let me know i’ll email you some simple letter cuts etc

Kev

[Gert du Preez]

The Sino machines usually comes with a rip-off / pirated software package, but the higher spec machines ship with UcanCam. (Domestic Chinese developed software)As far as I can gather this is not a rip off, and based on video tutorials etc. I saw, it looks like a decent package.

For sign work just about anything can work. Even flimsy DIY machines made with MDF and thread rod lead screws can outperform anybody with a manual jigsaw / palm router!

BTW, I run a fairly high spec pair of routers made by Tekcel in Australia. The big machine has very powerful dual vacuum, drawing through a sacrificial MDF sheet. Works a charm on big stock, but small stuff I still staple to the board.

Cutting 3mm Perspex, I find the perspex always "climbs up" on an upcut bit. I only use upcut bits, so the solution was to run 2 passes – the first 2.5mm deep (with 1 x 3mm tabs) and the second cut then plunges 3mm, but only cuts the 0.5mm remaining. (once again with 1 x 3mm tabs) Problem solved.

Getting a router to move is no more difficult than using a vinyl cutter. The skill comes in determining cut rates, DOC etc for the wide variety of materials you cut on these. Search the web, lots of info on this. DONT follow the lead of 95% of Youtubers. Those guys grind away with 2 flute cutters at 20k rpm at 6mm per sec with a DOC of 0,2mm 👿 Rather look for the info on the websites of good cnc router bit manufacturers. Start conservative, and work your way up to find the sweet spot of the machine. And please dont run the spindle at 24 000 rpm just because it can! I do most of my work (perspex, DiBond, Aluminium, MDF) at 12 – 15 000 rpm.

CNC routers are a hobby and addiction all on their own. I even started using the phrase "cnc perfect" since using them. Its so bad, that I neglect all other work in favour of cnc jobs! Then, when I get home, I tinker on my Isel router (standing in the dining room….on a cnc made table!) or I watch cnc video clips on the web, or browse cnc forums. It really is that much fun.

[David McDonald]

Kevin

Sincere thanks for your time on the phone earlier.

Having dusted off an old XP laptop we are connecting directly to the router/DSP and not using a USB stick for file transfer.

We can transfer files to the DSP Pendant and now the moment of truth we are going to actually get it cutting something!! (or skim the spoli board)

Thanks again Kevin – If we ever meet face to face I owe you a beer or more.

Cheers
Macky

[Kevin Flowers]

David
not a problem feel free to call anytime, have you got adjustable feet on your router if so ensure you level everything before skimming the spoil board, if you don’t have adjustable feet either add them or pack the legs to its level. I had problems with mine because it was didn’t have any adjusters so added these myself and depth is now a lot more accurate

Kev

[David McDonald]

Hi Kev

Thanks again ……. but one more question.

We have found that everything is out in scale by 60%

i.e. we have designed concentric rectangles to skim the bed with a 1" cutter. Its 1500 * 3050mm rectangle and then in-lined 30 or so times at 18mm intervals.

We then export it as a DXF file, millimetre units.

Take this file into Cut-2D, add the tool details and export as generic G-code (mm)

Copy this onto the DSP Pendant and set it off.

So everything should work fine but we kept getting over-X and over-Y error messages, i.e. trying to cut something bigger than the physical bed setting. We checked these X/Y ‘soft limit’ setup in the DSP pendant and everything is correct here.

After a little messing around we have deduced that the router ‘thinks’ it has a 600 by 1200 bed. If you manually move the X/Y is counts in increments 1-600 on the X, and 1-1200 on the Y. i.e if we cut a rectangle measuring 600mm * 1200mm it covers the whole 1500mm * 3050mm bed.

The workaround at the moment is for us to scale the DXF file down to 40% of its original size and now we are skimming the bed OK.

It’s going to be a pain having to scale everything we cut to 40%.

Any suggestions ? Is there a scaling option in the DSP pendant may be?

Cheers
Dave

[Kevin Flowers]

David
a few things to try
1. Don’t use DXF just export as a EPS and then import into Cut 2D, you can get issues with DXF and this may be your problem
2. In the pendant go through the different menu’s and you should find one that says table size check that this is set to the 3mtr x 1.5mtr
3. Try a different gcode engine i use (G Code ATC mm) if i remember correctly
4. It may also be that someone as adjusted the screw interspace but try the above first and let us know how you get on

Re skimming the bed just draw a rectangle to the size then use the pocket tool, next to the cutting tool icon this will then give you the option of either "Of Set" or "Raster clearance" pictures will show you the difference the reason for this is it will overlap (step over) its cutting as set up in the tool menu and give a better finish.

Kev

[David McDonald]

Hi Kev

Thanks again for your input.

I tried different export options and EPS rather than DXF but to no avail, your comment on interspace got me digging though – and I think I’ve cracked it with changing the ‘pulse equivalent’ setting.

It was set to its default at 320 p/mm, and I came across some info on a CNC site saying it should be 127.3 p/mm, which is almost to a fraction of a mm, the 60% difference in scale I was experiencing. Changed it to 127.3 and everything is now sized exactly right.

Got the spoil board nicely skimmed now (thanks for the comment on the pocket tool)

BUT – just one more question!

After cutting something the tool stays in the substrate at its final Z-depth, rather than lifting back out before traversing back to the origin. Dpending on what I’m cutting it ruins the piece.

I’m sure there must be a simple setting to change, most likely in Cut-2D, but after 3-hours still cant see it.

Any ideas?

(the pints I owe you are now up to a barrel)

Cheers
Dave

[Kevin Flowers]

David
yes pulse equivalent sounds right i was trying to remember the menu whilst sitting at home. Cut 2D his basically just a Tool path & Gcode generator when used in conjuction with these machines all settings are in the ontroller. Now you need to go back in to the settings on the controller, can’t tell you exactly where it is but there will be a command for it to return home. What i will say is that before you make any changes always make a note of original settings. It sounds like someone as had a good play with it or did something i did. Basically never use a really large usb compatible thumb drive cause it wipes the program out of the controller sorry forgot you are linking up to a pc for file transfer.

Just checked on mine it is Menu – System Menu – Function then scroll through and you should find home control

Hope this helps look forward to seeing some of the high quality work i know you are going to produce with it, don’t hesitate to contact me if i can help point you in the right direction on anything else

Kev

P.S
Have you sorted out how to get the machine to see its origin point rather that always starting from home position, how are you setting the Z depth, is the spindle set to run at 1 speed only or are you adjusting independently