New to shopbot And Aspire

[Nstep007]

Hi everyone, I acquired a Shopbot CNC last week, as well as aspire 8.0. I have been doing well in the program as far as designing. But when i go to cut the file, it will cut one tool path, return to home, and cut another... but then somehow it will start cutting something its not suppose to. Not sure what i am doing wrong... but most certainly am doing something. Any help would be appreciated. I tried to upload a pic, but having no luck

[srwtlc]

Really gonna need to have your file to look at to be able to help. Zip it up and post it if you can and it's not customer sensitive or copyrighted content.

What post processor are you using to generate your toolpaths? Some PP's will return to home at the end/start of each additional toolpath in a file.

[BrandanS]

Nick,

Post your response here (not the other thread); it'll get confusing. Scott and/or I will see what we can do once you've replied with your program with attached or copy and pasted.

Brandan

[Nstep007]

Will do, Thanks Brandan. Trying to get the code now, as i am using a different computer then i use for the Shopbot

[BrandanS]

Will do, Thanks Brandon. Trying to get the code now, as i am using a different computer then i use for the Shopbot

No problem, I'll keep checking back for your response.

Brandan

[Nstep007]

K. got the code. Tried to paste, but the forum says the file has too many characters. (23000) suggestion?

[Nstep007]

28670

28671

and just to note, i have tried to recreate and cut this design several times, and every time the machine does not cut it properly. And another note, i have to go into edit the code, I'm sure your will notice the MS 0.0,0.0 i have to manually change that to MS 2.5,0.6

[BrandanS]

28670

28671

Nick,

I've took a second to review your code and it does seem that Scott was right about the post processor being problematic. The Post Processor is what translates your ASPIRE Toolpath to the ShopBot Code. Choosing a functional one could save you alot of time.

I actually don't use Aspire myself, but I am sure there must be an appropriate post-processor in the software provided. Perhaps Scott, or another Aspire user could help here.

In the short term, I can help with the code you've posted. I was able to track down the places where the machine is going to it's 'home' position after it's completed it's toolpath.

The lines numbers 16, 1291, 2400, 3511 and perhaps 7008 (it's the last motion in the code; you may want the machine to go home at this point).

Again, this 'going home' action likely occurs at the beginning of a newly introduced toolpath and is being generated my your Post Processor.

Harder to track down, is the 'extra' machining wherein a radius is being machined right through your piece.

I previewed your program with ShopBot Control's Preview and it produced:

28672

I can't see where that extra radius is coming from so I'll need a bit more time.

[BrandanS]

Nick,

Perhaps you hadn't setup your post-processor, and that's where all these headaches are coming from.

Check this out from Vetric:

http://support.vectric.com/aspire-questions/item/how-to-find-the-correct-post-processor-for-my-machine

[BrandanS]

28670

28671

and just to note, i have tried to recreate and cut this design several times, and every time the machine does not cut it properly. And another note, i have to go into edit the code, I'm sure your will notice the MS 0.0,0.0 i have to manually change that to MS 2.5,0.6

This MS, 0.0, 0.0 would be generated from tool settings which must be defined within Aspire. I believe it's a table that look like:

28673

You'll want to define Feed Rate and Plunge Rate for your MS, 0.0, 0.0 issue.

[BrandanS]

I've dug a little further into your Post-Processor and found this:

http://forum.vectric.com/viewtopic.php?f=27&t=20615

Please note the date is 2014, but it should at least set you on the right path.

If you're confident with the post-processor, I was thinking that there "may" be an option in Aspire which will have the machine go home after each Toolpath has been completed. Maybe take a second to review and familiarize yourself with all the setup options you have available.

I am a SolidCAM user, but the theory is the same. I wish I used Aspire so that I could point out exactly what you needed to do.

Finally, while I have you on the line so-to-speak :D, make sure you reply back with your findings. ShopBot has an awesome community for support, and there are always people who have similar questions or suggestions. Writing back, saying what worked and what didn't, may help the next new user plagued with similar issues.

Brandan

[Nstep007]

Will do, i will try all of this soon. Now as far as my speed rates go, all that is set properly within the tool paths.... but yet it still always says MS0.0,0.0

Now forgive me for being lost on the Post Processor, What do i need to do to set that up?

[Nstep007]

When i save my tool paths, i save them as Shopbot(inch)(*.sbp) Why? i don't know, prolly watched a youtube video... Now i have went into the post prossecor and put Shopbot(inch)(*sbp) into MyPost_P.

28674

28675

28676

28677

[Joe Porter]

Nick, the post processor choices are in the drop down list under "Save Toolpaths" on the toolpath side of the screen. At the top of that pane is also a check box to "Output all visible toolpaths to one file", that is assuming you are using the same tool, which I think you are. I think most of us use the ShopBot, arcs in. with a standard machine and the Alphas use the PP "...with speed" added into it. I also noted that your cut speed or "Feed" is really slow, like 2.5" per Minute. I think you mean per Second? that's 150" per minute, which is a little fast if you have a Standard. Your plunge speeds are also set at .6" per minute. I see your design is in the lower left corner of the material, but the toolpaths are in the center. I don't know how that happened. Finally, the outer circle has a duplicate vector on top, that should be eliminated. I hope this has been of some help...joe

[srwtlc]

Nick,

You'll want to use the PP named (as it's named in the PP folder), ShopBot_Arc_Inch_Spindle_Control or ShopBot_Arc_Inch_Toolchange_Control if you have a toolchanger or utilize the manual toolchange method. If you don't intend to use the manual toolchange method, don't use that one. You could also try using the PP that is in your C:\SbParts\VCarvePro_forShopBotPosts folder called ShopBot_TC_inch (this one also handles arcs properly). I think that only this last one is configured properly to not return home upon start of each new section, but it may prompt you for tools and if you don't have tools numbered properly, it may also throw an error. Personally, I don't use that system and have customized my own PP to suit me. The change needed to stop the return home is easily done with any of the other PP's. Do you use a spindle or just a router? If a spindle, do you have the RPM controller (little dongle)?

For the (M)ove (S)peed being at 0,0, you need to set up your tool database so that all your tools have a feed and plunge value in in/sec and an RPM if you use a spindle with rpm controller. Once a tool is selected, you can also go to the edit button and adjust accordingly. In the case of your file, you will get an error that a parameter is wrong and it will set it to the lowest value allowed, which is going to be slow. Setting proper tool numbers would be recommended as well.

I ran your file in the SB previewer and I didn't see a stray cut. Where is it doing it? Maybe I just can't see it.

Could you possibly have changed the XY datum of your job after creating toolpaths and then not recalculate them. That would make it cut in the center of your job which could be way off from what you intended it to be as the pp processed the old toolpath with the new datum.

[Nstep007]

Scott, once i get ready to send the file to the production computer, i always recalculate tool paths

[Nstep007]

On the design tab, do i have to be aware of the layers?
Also, since all these cuts will be the same (pocket .125" deep into the wood) can i just select all the letters and make it 1 tool path? as well as the inner circle around the letters?

[Nstep007]

Nick, the post processor choices are in the drop down list under "Save Toolpaths" on the toolpath side of the screen. At the top of that pane is also a check box to "Output all visible toolpaths to one file", that is assuming you are using the same tool, which I think you are. I think most of us use the ShopBot, arcs in. with a standard machine and the Alphas use the PP "...with speed" added into it. I also noted that your cut speed or "Feed" is really slow, like 2.5" per Minute. I think you mean per Second? that's 150" per minute, which is a little fast if you have a Standard. Your plunge speeds are also set at .6" per minute. I see your design is in the lower left corner of the material, but the toolpaths are in the center. I don't know how that happened. Finally, the outer circle has a duplicate vector on top, that should be eliminated. I hope this has been of some help...joe
what would you recommend?
28678

28679

As well, as does the tool edit and the tool database have to match each other in the feeds and speeds?

[Nstep007]

Just a quick update guys. I made several cuts today successfully. Don't know how i can thank you all.

For future forum lookers, They main things i changed, was i added a Post Processor... the correct one. I changed my feed speeds, but most importantly i made sure i recalculated all my tool paths before i saved, as before i made sever changes and apparently moved stuff around. Hopefully i can get this whole CNC thing down and help someone in the future... Thanx again everyone... I'm sure you guys will hear from me soon ;)

[srwtlc]

At some point, your artwork was moved from where the toolpath was generated. If you tick on 'Show 2D previews' and check mark all toolpaths, you can see that the toolpath is in the center of your job dimensions. If you recalculate, it moves to where your artwork is. That may be the problem of going to where you think it shouldn't be going to.

If you are using layers, there's a chance that you may have a layer turned off that has some artwork that has a toolpath associated with it, or you may have some artwork that is on a bitmap layer that could be turned off. So, yes, one needs to be aware of layers if using layers. Grouping and ungrouping of vectors that may be on different layers can be confusing the first time it comes up.

You can do all the letters in one toolpath, but not the circle since that is a profile path and not a pocket.

As far as feeds and speeds, it will depend on what kind of machine you have, Standard or Alpha and if you are using a router or spindle. A good starting point might be around 12000 - 14000 rpm and 2 - 3 inches per second. If you have a router, you may not be able to run lower than 16000 and still have the needed torque for heavy cuts. These are just ballpark figures to start from.

I look at the tool database as suggested settings (according to what I have previously set them to) and once a tool is selected, I'll edit the settings to match the task at hand. If I think it needs to be slower, faster, more depth per pass, etc., that's where I do that. So, no, they do not need to match.

Because you feed settings are so slow and in in/min, when converted to in/sec by the PP, the values are so small that they are just calculated to 0. Set your feeds to inches per second and enter something like 2.5 and 1 and the PP will assign the proper feedrates then.

If you need some help with modifying the PP so it doesn't return to home each time and so it doesn't do the gradual ramp downward on it's way to the start of the cut, we can work that out.

Edited after seeing your last post to say....Good, glad you got it worked out!

[Nstep007]

Scott, Huge thanks to you for your help. Appreciate everyone taking time out of their day to assist me. Yes, would like to make it where it doesn't return home everytime

[BrandanS]

Scott, Huge thanks to you for your help. Appreciate everyone taking time out of their day to assist me. Yes, would like to make it where it doesn't return home everytime

Nick,

Glad to see you got it going after all. Thanks for posting your results!

Brandan

[Nstep007]

Hi everyone, Hope all is well. After i was able to cut my sign last week, this week i am having the same exact problem. But now, for some reason last night, the Z axis went all the way down at some point, did not move back up, and while this happened the machine wanted to travel on the x and y axis, which made the gantry jump off of it tracks.... now the machine is not only cutting in odd places... but now it is cutting jagged... i was able to get the gantry back on track, not sure id there is a alignment thing I'm suppose to do. Im lost and discouraged at this point, but trying my hardest not to give up. If you can help me with anything id appreciate it. I attached the file i was cutting, a picture of the shobot, as well as a pic of the board i was cutting.

28694

28695

28696

[Nstep007]

Update: I think i have found my problem... When i was moving the X & Y axis with the keyboard, i noticed it would move rather slow... compared to when i would hit the "jog home" button. e When it would go home, i noticed at some point, the gantry would seem like it was getting tangled up, not in any particular place as to where the spindles might have been broke, but every time it would "kink" up in different places.... So apparently when the CNC would make a Cut, and it would go home... it was traveling home way to fast, and would slightly "Kink Up". So i slowed that down from 12.0 to 3.0 and have not had any problems since... Im sure this is a older model and that rail system I'm sure has been upgraded simply for this reason.... huge relief... still have a lot to learn