Cut Tolerances With Fusion

[dbchaplin03]

This is my first post and I am brand, brand new to this forum and CNC Plasma cutting in general. Haven't pulled the trigger on a plasma table just yet but am reading tons of posts on here to help decide which one would be best for me (I am planning to place the order within the next month or so). I have many years of tinkering and fabrication as a hobbyist. Grew up on a farm and have spent the last 20+ years in the Air Force. I'm retiring in a couple years and am starting a part time fabrication business that i hope to do full time when I retire from active duty.

One of my first big projects is going to be a slot and groove welding table similar to the certiflat or the DXF files by Makers Table. I have been teaching myself, with the help of youtube, how to design and model in Fusion 360.

My question is this: Do I build tolerances into my Fusion drawings, or are the tolerances added in the g-code/cutting software? Makers Tables for example says he builds in .03" of tolerance to compensate for plasma cutters being less accurate than a laser. I just don't know if I build that into each hole or joint in Fusion or if that will be a setting when you go to cut it?

So for example if I do a hole I've been making a 5/8" hole, 5/8+.03 = .655". Or a 1" slot in 1/4" material I've been making 1.03" x .28" to compensate.

I know that some trial and error will be needed once i take delivery of the machine before I start cutting full 4x8 or 5x10 sheets of steel plate and wasting money but since I'm learning the software by designing projects, i just wanted to get the basic tolerances correct. I'm also designing a press brake, log splitter, and a few other things.

Thank you so much for any help you offer. I really enjoy this stuff and look forward to this next journey into CNC cutting.

[weldguy]

Welcome to the site, sounds like you have a great plan when you retire and I thank you for your service.

Great question and the answer is to design the parts to the actual desired finished size. When you are done designing and you run that design through your post processing software to generate the g-code it will create the offset in your cut path to compensate for the kerf width.

What tables are you looking at possible buying?

[dbchaplin03]

Thank you so much for your advice! That will help a ton when it comes designing some of these projects. I'll need to go back into a few of them to adjust the tolerances.

For tables I've been looking at Langmuir, STV, ARClight, ShopSabre, and a company called LDS CNC. I've also seen a couple of Torchmate and one ShopSabre for sale on Marketplace as turn key packages with the plasmas as well that I've considered.

[tcaudle]

The tolerance of a cut is in the machine cutting it . It's a combination of Resolution, backlash, non-linear mechanics and fitment. Few plasma tables can hold anywhere near the Resolution number (smallest distance per digital Step) listed as opposed to all of the other errors inherent in the system.
Then, even if you get to a point the final motion ACCURACY is say ,005, you have to deal with the whole Plasma variables. The kerf width of a plasma cut is dependant on several things: The orifice diameter of the nozzle (that wears over time) , the air pressure and quality of air (dry and clean) , the height of the cut *arc gap") and the feed rate. Slower feed rates will cause wider kerfs . Bottom line if you can hold +or- .010 its a very tight cut. That means a hole could be out as much as .020 overall . You don't use plasma for high tolerance cuts If you need exact dimension pieces you mark and drive or machine them. Plasm cuts are not perfectly stright sided cuts they tend to flare from top to bottom

Plasma is great for cutting material for weldment fabrication , parts that do not have to fit precisely to other parts and for doing decorative cutting.

Most of the brands you listed all use different software, different controllers , different THC's. Some use All-in-One CAD/design and CAM tools . it's faster (maybe) to learn, but you may find one or more of the tools might not have the features you want. There are things you won't learn about until the table is in your shop and you are trying to make it cut. One of the top selection criteria for a commercial table needs to be the level of support you can get (you will get NONE on a used table ) A lot of the systems you see for sale are old and obsolete. You can't get help and you can't get repair parts. You are stuck with upgrading/rebuilding or selling it to the next sucker.

The other thing to consider is the ability to add features and options at reasonable prices. While all you may ever want to do is cut flat metal, its nice to at least have some options available:
Rotary Cutting (pipe and tubing) Round and square. Support for separate controller rotary axis.
Plate markingusing pneumatic marking tool . Ability to combine marking with plasma cutting in same cut file.
Compatible Hand controller Wired or WIFI ....NO Bluetooth!
Net-workable control computer to be able to send files via Ethernet or WIFI.
Oxy - Fuel Support (manual THC and added outputs for valves and solenoids).
Support for (gasp) router or rotary cutting tools. Means full 3 axis with Full active Z axis .

There are some more but all these vary with he vendor and model of controls.

While Fusion 360 is a good CAD and even better 3D design tool, its CAM for Plasma is rather limited . Its a lot of money to pay (every month) to do 2D cutting, Before the screams of "Free Version" are mounted, read the license file restrictions and discover "hobby" means largely a Not-for-profit application or individual use for fun.

At one time it was easier to pick out a Plasma table, There were only a hand full of vendors. Now everybody and their dog has a table for sale. You typically can't get enough information off their website to figure out much of the technology . Even if you can, its confusing. Most vendors list "automatic torch height " as a button feature (like "power brakes") and that can mean anything from a slow stand-alone controller with knobs and buttons to set for each cut, all the way to full auto "in-motion, closed loop" designs .

[adbuch]

My question is this: Do I build tolerances into my Fusion drawings, or are the tolerances added in the g-code/cutting software? Makers Tables for example says he builds in .03" of tolerance to compensate for plasma cutters being less accurate than a laser. I just don't know if I build that into each hole or joint in Fusion or if that will be a setting when you go to cut it?

When you draw your parts in Fusion 360, draw them to the size you want them. If you have a tab that fits into a slot and you want the slot to be wider than the tab by 0.030", then draw the slot so that the width is 0.030" wider than the tab that will fit into it. When actually cutting your parts, you will need to do a test cut (say a straight line 6" long) and measure the actual kerf width of this line. Then enter that value into your cam or control software so that the resultant g-code will compensate for the kerf width. Finally cut a test part - say a 4" square - and measure the finished dimensions to see how closely they match the actual 4" dimensions of your drawing (dxf file). Then if necessary, adjust the kerf width setting in the cam or control software and repeat the test cut and measure again. Once you have your kerf width setting "dialed in" - you should be able to achieve a final cut dimension of 4.000" plus or minus several thousandths of an inch. I achieve those sorts of results with my Plasmacam DHC2 /Hypertherm PM 80 combination.

Here is an example of a part I cut from 11 ga. steel. As drawn, the part is 4.750" OD with a 0.750" ID hole. The actual finished dimensions (as cut) are marked onto the top of the part.

David

text cut.jpg

[dbchaplin03]

David,

Thank you very much for the thorough response. Is it safe to assume I would need to find this Kerf width for different thicknesses or does it stay consistent? The first several projects I have planned will use 1/4, 3/8, and 1/2" material.

I plan to order my table with either a Hypertherm Sync 65 or 85. I sold my 45 XP because it was an older model and didn't have the serial port.

[adbuch]

David,

Thank you very much for the thorough response. Is it safe to assume I would need to find this Kerf width for different thicknesses or does it stay consistent? The first several projects I have planned will use 1/4, 3/8, and 1/2" material.

I plan to order my table with either a Hypertherm Sync 65 or 85. I sold my 45 XP because it was an older model and didn't have the serial port.

The kerf width will be dependent on material thickness, current setting (amps), and type of consumables used. Here is the estimated kerf width compensation chart for the Hypertherm PM85 with Duramax torch. This is one of the plasma cutters I use, along with the Hypertherm 45xp.

My plasma cutters are the non-sync versions with no CPC port. The CPC port would be required for machine torch application. I am using a hand torch with the torch control cable hard wired to the plasma cutter.

The values for kerf width in the chart are only estimates. For best results, do a test cut for the setup (or setups) you intend to use and measure the actual kerf width.

David

Kerf width chart.jpg

[adbuch]

Here is an example of a simple plate with hole drawn with Fusion 360. After you have cut a test part, you could measure the finished dimensions of the part and adjust your kerf width setting accordingly. I would still recommend cutting a straight line first and measuring the kerf width as I suggested previously. Then use this value as your starting point in your Fusion 360 program.

David

1.jpg

2.jpg

3.jpg

[cuttinparts]

Awesome info David, thanks!

[adbuch]

Awesome info David, thanks!

You are quite welcome!
David

[tcaudle]

I plan to order my table with either a Hypertherm Sync 65 or 85. I sold my 45 XP because it was an older model and didn't have the serial port.

By serial port are you referring to the 14 pin CPC connector or the RS485 5 wide serial port ?

If it's the latter you will find there are not a lot of tables/controls that support the actual Hypertherm Serial (RS485) port.

FYI the RS485 Serial Port is used to remotely set the cut current and air pressure from software. It offers some features taht you can't do with manual adjustment. One is the abiliyt to do a "soft piecre" . Its the process of starting a pierce at a lower power (amps) and slowing down the plunge to cut height and ramping the amps to full at the bottom. it has proven to increase consumable life and cause less back splash and damaged shields . It works best on material thicker than 11 Ga. Also works well to do "center pecking" to do a non-penetrating divot at the center point of holes to be drilled rather than a full pierce and the ragged and hardened hole that leaves..

[plasmanewbie]

Very interesting Tom, I had no idea the serial port offered that ability. Thanks for the great read.

[djreiswig]

The serial port also returns error messages from the Hypertherm to the computer.

[tcaudle]

It is less useful on say a 45 series than a 65/85/125 that has a much wider range of cut current settings . Hypertherm is the only manufacturer to offer the RS468t interface option and its available as an option on order of the unit or you can add it in the field. its a couple of connections and a connector added to a cut-out on the back. And yes, it reads output from the plasma of which one are the error messages from the unit. They are codes you have to look up in the manual BUT our software does that for you and puts them in plain language..

The serial port just gives you the tools and parameters . Its up tot he software and the CAM program to make it useful. Changing settings dynamically (on the fly) has to be done in real time from g-code. Once its in the g-code it happens every time its run . The problem with a lot of POST processors is they do not allow for "logic" or declared variables. Things like " IF this variable is equal to or greater than another , THEN do this/
..." type stements. So you can trigger events based on the feedback .

[dbchaplin03]

I’ve got so much to learn ! Thank you all for the feedback and knowledge.

[adbuch]

I’ve got so much to learn ! Thank you all for the feedback and knowledge.

When you said "serial port" - were you referring to the CPC connector which is required for machine torch operation, or were you actually talking about a serial port as described by tcaudle? These are two entirely different things.

David

[dbchaplin03]

I meant the CPC connector.

[dbchaplin03]

I have one other super newby question for you guys. I don't buy many full size sheets of plate because I've never had CNC so i mostly cut leftover pieces or buy drops from the steel supplier.

Is a 4x8 sheet of plate actually 4x8 or do the dimensions vary like lumber? The reason I ask is because I'm designing a 4x8 table because it makes it much easier to design with the tab and slots. This table is the only thing I can think of that I'll cut that close to the size of a full sheet but I'm not sure if I can actually cut it out of a 4x8 or if I would have to go up to a 5x10. That decision plays into whether or not I should consider a 4x8 vs a 5x10 table as well. I'm leaning towards the 4x8 to save shop space but I also don't want to regret buying one too small. Any advice is also appreciated.

[adbuch]

I meant the CPC connector.

[adbuch]

I have one other super newby question for you guys. I don't buy many full size sheets of plate because I've never had CNC so i mostly cut leftover pieces or buy drops from the steel supplier.

Is a 4x8 sheet of plate actually 4x8 or do the dimensions vary like lumber? The reason I ask is because I'm designing a 4x8 table because it makes it much easier to design with the tab and slots. This table is the only thing I can think of that I'll cut that close to the size of a full sheet but I'm not sure if I can actually cut it out of a 4x8 or if I would have to go up to a 5x10. That decision plays into whether or not I should consider a 4x8 vs a 5x10 table as well. I'm leaning towards the 4x8 to save shop space but I also don't want to regret buying one too small. Any advice is also appreciated.

The 4 x 8 sheets I buy are actually 48" x 96" in size. I usually have them cut in half for easier handling.
David

[djreiswig]

Sometimes the full sheets I buy are 1/8 to 1/4 oversized. It varies. If you're going to be cutting full sheets, make sure you have extra travel on your table so the torch and any accessories can reach the entire sheet. I wish mine was a bit wider so my air scribe would reach to both edges. Not a huge deal, since I don't use it much. Just have to remember when I place the material.