[DontBeLate]

Boy, while the concepts of setting feed rates and cutter speeds are straightforward enough, actually nailing down the numbers to program into the bobcam tools is a surprisingly murky matter involving a myriad of inter-related factors that are inconsistently used across CAM tools and in how to guides. It makes me wonder if I'm doing it right and wanting to get a single documented process in place. It seems most materials and cutters have been around long enough for a standard table to have been generated for at least a starting point with fine tuning for faster production once milling begins.

Can someone check my process here and/or suggest a tool or table that supports wood and plastics?

My V24 (yes I know I'm far down rev but I'm not a production shop) tools allows assigning
Z Plunge Feed/Small Tool sf ft/min and in/tooth per material type for

End Mill Rough
End Mill Finish

XY traverse Feed / Large Tool sf ft/min and in/tooth per material type for

End Mill Rough
End Mill Finish

The BOBCAM software then calculates the feed rates and spindle speeds for the operation being performed. What is confusing is that I specify/calculate these feed rates and spindle speeds so I can calculate the sf and in/tooth factors but the feed rates and spindle speeds calculated by the BOBCAM tool do not match as if they are being adjusted by the BOBCAM tool on a per operation basis.

Getting to these numbers I've had to hop around finding calculating tools and formulas on various web sites and documents. Not finding a cohesive process and calculation tools makes me wary of the results I'm calculating.

Here are the steps I've followed:
1. Determine the appropriate chip load for the material being cut (currently hardwood plywood):
Chiploads | Feeds and Speeds | Metal | Plastic | Composite | | Documents
Apache Tomcat/6.0.44 - Error report

2. Determine the Feed Rate
Using a formula found in this document:
http://www.shopbottools.com/files/SB...%2011%2003.pdf

Feed Rate (IPM) = RPM x # of cutting edges x Chip Load

3. Calculate the In/tooth using the calculators from either of these web sites
Speeds and Feeds Calculator
https://www.carbidedepot.com/formulas-milling.htm

This is all just to get a starting point to get on to the Shopbot CNC router. I expect once I cut a few test cuts I'll have to adjust the feed rate and spindle speed to optimize the chip size so I can get the smoothest finished edge

[The Engine Guy]

I see you have done all the usual research where you end up with a huge headache, what you have is as much as you will ever find IMHO, my advice is to start with the cutter manufacturers, supply them with details of your machine, clamping system and materials to be cut, they will be able to give you proper speed and feed information for their product

Most manufacturers I have found are very helpful, sometimes they even get a rep to call in at the shop with his magic book of numbers, couple of times I have even got a cutter to try out for free

Always worth a try

Regards
Rob
:rainfro: :rainfro: :rainfro:

[jrmach]

this is where there is no substitute for experience

the variables are enormous

What are you cutting with what machine ?

[DontBeLate]

Thank you guys for the replies.
Yes a giant hairball from a newbie perspective and it's not helping bobcam seems to want what seems like uncommon factors as part of the setup.

I thought I'd start off easy using hardwood plywood
Buy Baltic Birch Plywood 3mm-1/8" x 30" x 48" at Woodcraft.com

Some spiral upcut bits from whiteside
Buy Whiteside RU1600 Solid Carbide Spiral Upcut Router Bit 1/4" Sh 1/8" D 1/2" CL 2" OL at Woodcraft.com

Bobcam V24

Shopbot Alpha
PRSalpha CNC Routers

Once I have all the parts coming out right I'll migrate to hardwoods.

[mmoe]

Thank you guys for the replies.
Yes a giant hairball from a newbie perspective and it's not helping bobcam seems to want what seems like uncommon factors as part of the setup.

I thought I'd start off easy using hardwood plywood
Buy Baltic Birch Plywood 3mm-1/8" x 30" x 48" at Woodcraft.com

Some spiral upcut bits from whiteside
Buy Whiteside RU1600 Solid Carbide Spiral Upcut Router Bit 1/4" Sh 1/8" D 1/2" CL 2" OL at Woodcraft.com

Bobcam V24

Shopbot Alpha
PRSalpha CNC Routers

Once I have all the parts coming out right I'll migrate to hardwoods.

As a starting point, you'll want to run at around 50 ipm with 15000 rpms to cut that material with a 1/8 inch router bit. No need for multi passes in depth. Just run full depth, conventional milling, not climb milling.

Cuts about the same as hardwood since it is essentially layers of hardwood. I would recommend down spiral over up spiral. Baltic Birch splinters more at the top with up shear.

[DontBeLate]

Ok
mmoe,
So your advise is to not bother entering the SFM and in/tooth values into the settings for each material and to not use the system calculated values for feed and speed. Correct?
Then, every time I specify an operation I uncheck the "Use System Feeds and Speeds" and manually enter these values in the feeds and speeds section
Spindle RPM = 15000
Cutting Feed Rate = 50 - (IPM?)
Plunge Feed Rate = 50? - (IPM?)

One thing that is lacking is that there are no units specified in Bobcam for any of these manually entered parameters.
I'm looking to verify the units because when I use the ShopBot_sbp_Rev12.MillPst it generates a code line of "MS,50.". When loading this into the shopbot control software I get an error indicating this value is too large and it resets it to the maximum value of 12. So either the shopbot control software has been limited to only accept feed rates of 12 IPM
or
the shopbot control software is expecting IPS and either the Bobcam post processing script has a scaling problem or the units that are entered in the feeds and speeds section are really IPS instead of IPM.

Can anyone shed some light on this?

[BurrMan]

The system setup is more an automated way to set yourself up.. it works fine, its just not overly "robust" when you really want to dig into controlling this area.

Bobcad has a machinist toolbox for this. More didicated to that area. I think jrmach has anotherone he likes that a guy sells.

[mmoe]

Ok
mmoe,
So your advise is to not bother entering the SFM and in/tooth values into the settings for each material and to not use the system calculated values for feed and speed. Correct?
Then, every time I specify an operation I uncheck the "Use System Feeds and Speeds" and manually enter these values in the feeds and speeds section
Spindle RPM = 15000
Cutting Feed Rate = 50 - (IPM?)
Plunge Feed Rate = 50? - (IPM?)

One thing that is lacking is that there are no units specified in Bobcam for any of these manually entered parameters.
I'm looking to verify the units because when I use the ShopBot_sbp_Rev12.MillPst it generates a code line of "MS,50.". When loading this into the shopbot control software I get an error indicating this value is too large and it resets it to the maximum value of 12. So either the shopbot control software has been limited to only accept feed rates of 12 IPM
or
the shopbot control software is expecting IPS and either the Bobcam post processing script has a scaling problem or the units that are entered in the feeds and speeds section are really IPS instead of IPM.

Can anyone shed some light on this?

No matter how you set up the tool in Bobcad or any other cam system, you are only going to get a baseline feed/speed autofilled. You still have to apply judgement for a specific job or material and adjust, so no matter what you do, you need manual input either way. In some small portion of cases, it will be correct as is, but I know I always have a specific idea in mind and verify whether or not it's already correct.

I recall someone having an issue of ips vs. Ipm with fusion a while back as well. In bobcad, you can adjust the feed rate by adjusting the value in the post with math. Or, you can just enter ips into the box that should be ipm if you want to enter it the same way the controller wants it.will work either way. It is ipm in Bobcad if you are in inches.

[jrmach]

the one I like is Advanced CNC Speed And Feed Machinist Calculator - HSMAdvisor

But it is not for wood

mmoe should be the one to listen to here

[DontBeLate]

Thanks BurrMan
I'm having trouble getting the system setup to work considering the problems I stipulated. Having these baseline values auto calculated should be just fine for me considering I'm not doing production. Or perhaps this is a flawed assumption.

From what I've see on the standard formulas for
SFM = (RPM*Cutter Diameter in inches*(3.14159/12))
in/tooth = IPM / RPM / # of flutes
does not take the material into account even though it is being assigned on a material by material basis in Bobcam. Am I missing something here?

I figure Bobcam is adjusting the feeds and speeds based on the cutter specification and perhaps by the machine identification.

[DontBeLate]

So I've learned that the Shopbot is looking for IPS not IPM.
I went into the ShopBot_sbp_Rev12.MillPst and changed

line 217. Scale factor for feedrate? 1
to
217. Scale factor for feedrate? 0.016667

[Idiod]

Thanks BurrMan
I'm having trouble getting the system setup to work considering the problems I stipulated. Having these baseline values auto calculated should be just fine for me considering I'm not doing production. Or perhaps this is a flawed assumption.

From what I've see on the standard formulas for
SFM = (RPM*Cutter Diameter in inches*(3.14159/12))
in/tooth = IPM / RPM / # of flutes
does not take the material into account even though it is being assigned on a material by material basis in Bobcam. Am I missing something here?

I figure Bobcam is adjusting the feeds and speeds based on the cutter specification and perhaps by the machine identification.

I don't know what the value is for wood, but the formula to find RPM is: π x 12 ÷ Cutter Diameter x SFM. Surface feet per minute is the factor that takes into account material being cut as well as the Cutter material. The machinist handbook has the value for SFM for a lot of materials (mostly metal) I don't know if it has wood. After you find the correct RPM, then you can use: Ipm = RPM x Chip load per tooth x # of cutting edges. I hope this helps.

[jrmach]

So I've learned that the Shopbot is looking for IPS not IPM.
I went into the ShopBot_sbp_Rev12.MillPst and changed

line 217. Scale factor for feedrate? 1
to
217. Scale factor for feedrate? 0.016667

On Mills Inch Per Minute is widely preferred
On Lathes Inch Per Revolution
What is "IPS" ?

I would think there would be a parameter setting on your machine to change to IPM,,maybe ???,,,don't know your machine

[mmoe]

On Mills Inch Per Minute is widely preferred
On Lathes Inch Per Revolution
What is "IPS" ?

I would think there would be a parameter setting on your machine to change to IPM,,maybe ???,,,don't know your machine

I think Shopbot is the only machine I've run across that uses IPS (inches per second). This isn't the first time I've helped a shopbot user figure out how to deal with this somewhat unique approach, but I've never encountered it in any other commercially available machine.

[mmoe]

So I've learned that the Shopbot is looking for IPS not IPM.
I went into the ShopBot_sbp_Rev12.MillPst and changed

line 217. Scale factor for feedrate? 1
to
217. Scale factor for feedrate? 0.016667

If you plan to do your feedrates in the CAM software using inches per minute, this is the way to go. Enter your IPM when setting up the tool and it will get adjusted to IPS in post.

I've heard some prefer to use IPS over IPM, If that's the case, then leave the post processor alone and just enter the IPS value where it should be IPM. Since the value you enter is actually IPS, then not scaling the feedrate in the post processor would result in the correct feedrate. There is no option to enter IPS in Bobcad that I'm aware of (this is common for most CAM systems), so if you want to enter IPS, you have to just pretend it's IPS and make no conversions. The code will end up correct.

If it were me, I'd stick with IPM and adjust the post processor as you have. If you have conversations with other Bobcad users, no one else will be talking in terms of IPS, so it's probably best to stay with convention. It's hard enough when you have some of us using metric and some using inches without throwing subcategories of each in there!

[jrmach]

I think Shopbot is the only machine I've run across that uses IPS (inches per second). This isn't the first time I've helped a shopbot user figure out how to deal with this somewhat unique approach, but I've never encountered it in any other commercially available machine.

I can't imagine why they would,,must be something to do with the China electronics ???????

I would never like that

To the OP,,,if mmoe is indeed correct,,,you will have to go thru and change your feeds,,,,,,,,,,,,,,,I would imagine divide by 60

If your machine uses rpm you should be good with speeds

However,,,there are variables like the machine,etc. that only make the data base a starting point..With that machine I would be conservative until you get some hours of experience in to help nail down the optimum feeds and speeds

[BurrMan]

I can't imagine why they would,,must be something to do with the China electronics ???????


To the OP,,,if mmoe is indeed correct,,,you will have to go thru and change your feeds,,,,,,,,,,,,,,,I would imagine divide by 60

If your machine uses rpm you should be good with speeds

However,,,there are variables like the machine,etc. that only make the data base a starting point..With that machine I would be conservative until you get some hours of experience in to help nail down the optimum feeds and speeds

It is setup that way with shopbots. Sfs. So he has the right solution with setting the scale factor in his post. Because bobcad is an sfm system, he will enter those in his tools as sfm... so, setting up the tooling, if he is given sfs, he will need to convert his numbers to enter. If he is using sfm with his tooling, they will be converted down during posting fir the machine.

i think hes got that part now. Seems to be questioning whether the system will output the correct numbers per what he sets at the tool library level.

[Beansdiesel]

G-wizard has some wood in there for materials. This is what it comes up with with plywood as the material.Attachment 303276

If I put the finish setting down to "Fine Finish" the feed drops down to 17IPM, big drop, doesnt seem right. I wold guess somewhere in between there wold be a good place to start. Its wood so its pretty forgiving if you are off some.

x2 on the down spiral especially with that thin stuff.

You should download G-wiz, its free to try out for a month. Comes in really handy for me.